centroid M400, M39 Operators Manual

Download

Page 1

Centroid M-Series Operators Manual

CNC Software version: CNC11 V.3.12 Models: M400 & M39

M400 & M39

Operators Manual

Introduction

Operators Panel

Main Screen

Part Setup

Tool Setup

Running a Job

Utility Menu

Digitizing

Probing

1-1

2-1

3-1

4-1

5-1

6-1

7-1

8-1

9-1

Intercon Conversational Programming

www.centroidcnc.com

CNC Program codes

G- Codes

M code functions

Conguration

CNC Software Messages

10-1

11-1

12-1

13-1

14-1

15-1

Page 2

READ THIS MANUAL BEFORE USING THIS PRODUCT.

FAILURE TO FOLLOW THE INSTRUCTIONS AND SAFETY

PRECAUTIONS IN THIS MANUAL CAN RESULT IN

SERIOUS INJURY OR DEATH.

All operators and service personnel must read this manual before operating

CENTROID CNC control equipment and all connected machine tools.

Keep this manual in a safe location for future reference.

Throughout this manual and on associated products where applicable, in accordance with ANSI Z535, the following symbols and words are used as defined below:

DANGER

WARNING

CAUTION

NOTICE

Information provided by CENTROID relating to wiring, installation, and operation of CNC components is intended as only a guide, and in all cases a qualified technician and all applicable local codes and laws must be consulted. CENTROID makes no claims about the completeness or accuracy of the information provided, as it may apply to an infinite number of field conditions.

“DANGER” with or without a red background = Hazard WILL cause death or serious injury if ignored.

“WARNING” with or without an orange background = Hazard COULD cause death or serious injury if ignored.

“CAUTION” with or without a yellow background = Hazard MAY cause minor to moderate injury if ignored.

“NOTICE” with or without a blue background = Indicates an action to prevent damage to the product or other materials used with product.

As CNC control products from CENTROID can be installed on a wide variety of machine tools NOT sold or supported by CENTROID, you MUST consult and follow all safety

instructions provided by your machine tool manufacturer regarding the safe operation of your machine and unique application.

Page 3

CENTROID CNC controls provide facilities for a required Emergency Stop circuit which can be used to completely disable your machine tool in the event of an emergency or unsafe condition. Proper installation of your CNC control MUST include the necessary wiring

to disable ALL machine tool movement when the Emergency Stop button is pressed.

This includes machine, servo motors, tool changers, coolant pumps, and any other moving parts. DO NOT disable or alter any safety feature of your machine or CNC control.

Never alter or remove any safety sign or symbol from your machine or CNC control components. If signs become damaged or worn, or if additional signs are needed to

emphasize a particular safety issue, contact your dealer or CENTROID.

CNC Control Operating Specifications

Minimum Maximum

Operating Temperature 40°F (5°C) 104°F (40°C) Ambient Humidity 30% relative, non-condensing 90% relative, non-condensing Altitude 0 Ft. (Sea Level) 6000 Ft. (1830m) Input Voltage (110, 220, 440 VAC,

System Dependent)

Note: Your machine may have operating conditions different than those shown above. Always consult your machine manual and documentation.

-10% of Specified System Input Voltage

+10% of Specified System Input

Voltage

Safety signs and labels found on your machine tool, and on CNC system components typically follow the following examples:

Page 4

CNC Machine Tool Safety

•All machine tools contain hazards from rotating parts; movement of belts, pulleys, gears, and chains; high voltage electricity; compressed air; noise; and airborne dust, chips, swarf, coolant, and lubricants. Basic safety precautions must be followed to reduce the risk of personal injury and property damage.

•Your local safety codes and regulations must be consulted before installation and operation of your machine and CENTROID CNC control. Should a safety concern arise, always contact your dealer or service technician immediately.

•Access to all dangerous areas of the machine must be restricted while the machine is in use. Ensure

that all safety guards and doors are properly in place during use. Automatically controlled machine tools may start, stop, or move suddenly at any time. Do not enter the machining area when the machine is in motion; death or severe injury may result.

•Personal protective equipment, particularly ANSI-approved impact safety glasses and OSHAapproved hearing protection must be used. Proper handling, storage, use, and disposal of materials in accordance with manufacturer's instructions and Material Safety Data Sheets (MSDS, or your local equivalent) must be followed.

•DO NOT operate your machine or CNC control in explosive atmospheres or in environmental

conditions outside of the manufacturer's specified ranges. Electrical power must meet the specifications provided by your machine and CNC control manufacturer.

•DO NOT operate your machine or CNC control if any safety systems are damaged or missing. Excessively scratched or damaged windows and guards must be replaced.

•ONLY authorized personnel should be allowed to operate the machine and CNC control. Improper operation can cause injury, death, and machine or control damage, and may void applicable warranties.

•All electrical enclosures and panels MUST be closed and secured at all times except during installation and service. Only qualified electricians and service personnel should have access to these locations. Hazards arising from high voltage electricity and heat exist in the control cabinet, and may exist even after the main disconnect is turned OFF.

•Improperly clamped or fixtured parts; improperly secured tooling; and broken parts, fixtures, and tooling resulting from machining operations at unsafe feedrates and speeds may result in projectiles being ejected from your machine, even through safety systems such as guards and doors. Always follow safe and reasonable machining practices and follow all safety precautions provided by your tooling and machine manufacturer.

•Ultimate responsibility for safe operation and maintenance of your machine and CNC control rests with shop owners and machine operators. Before performing any work or maintenance all individuals should be thoroughly acquainted with the safe operation of BOTH machine tool AND CNC control.

•Shop owners and operators are responsible for ensuring that shop and machine safety systems such as Emergency Stop and fire suppression systems are present and functioning properly, as required by local codes and regulations.

Page 5

CNC Control Warning Labels

High Voltage Electrocution Hazard.

Death by electric shock can occur.

Turn off and lock out system power before servicing.

High Voltage Electrocution Hazard.

Death by electric shock can occur.

Turn off and lock out system power before servicing.

Page 6

TABLE OF CONTENTS

CHAPTER 1 - Introduction

Window Description 1-1 Conventions 1-3 Machine Home 1-4 Mill M and G Codes 1-5 Software Unlocks 1-6

CHAPTER 2 - Operator Panels

M-Series Jog Panel 2-1 Keyboard Jog Panel 2-5 Keyboard Shortcut Keys 2-7

CHAPTER 3 – CNC Software Main Screen

Option Descriptions 3-1

CHAPTER 4 - Part Setup

Operation Description 4-2 Part Setup Examples 4-4 Work Coordinate Systems Configuration 4-6 Coordinate Systems Rotation 4-7 Transformed WCS 4-8

CHAPTER 5 - Tool Setup

Offset Library 5-1 Automatic Tool Measurement 5-3 Setting up Tool Height Offsets 5-4 Tool Library 5-5 Tool Life Management 5-7

CHAPTER 6 – Running a Job

Job Run Screen with G-code Display 6-1 Run-Time Graphics 6-2 Canceling a Job in Progress 6-2 Resuming a Canceled Job 6-3 Run Menu 6-3 Power Feed 6-5

CHAPTER 7 - The Utility Menu

F2 – Update, F3 – Backup, F4 – Restore 7-1 F5 - File Ops. 7-2 F6 – User Maint, F7 – Report 7-3 F8 – Options, F9 – Logs 7-3

CHAPTER 8 – Digitize

Grid Digitize 8-2 Radial Digitize 8-6 Contour Digitize 8-10 Wall Following Digitizing 8-13 Dig to CAD 8-15

CHAPTER 9 - Probing

Part Setup with Probing 9-1 Calibrating the Probe Tip Diameter 9-2 Probing Cycles 9-2 Probe Parameters 9-7 DSP Probe Parameters 9-8

CHAPTER 10 - Intercon Software

Intercon Main Screen 10-1 File Menu 10-2 Rapid Traverse 10-7 Linear Mill 10-8 Arc Mill 10-10 Tool Functions 10-12 Canned Cycles 10-13

Drilling 10-16 Chip Breaking 10-17 Deep Hole Drilling 10-19 Boring 10-20 Tapping 10-22 Facing 10-24 Rectangular Pocket 10-25 Circular Pocket 10-27 Rectangular/Circular Frame Milling 10-29 Thread Milling 10-31 Cleanout 10-33

Subprograms 10-36

Repeat to Depth 10-38 Repeat 10-39 Mirror 10-40

Rotate 10-41 Graphics 10-42 Math Help 10-45 Importing DXF files 10-52 Intercon Tutorials 10-59

CHAPTER 11 – CNC Program Codes

Miscellaneous CNC Program Symbols 11-1 User and System Variables 11-5 Advanced Macro Statements 11-8

CHAPTER 12 - G-codes

G-Code Quick Reference 12-1 G-Code Descriptions 12-2

CHAPTER 13 - M functions

M function Quick Reference 13-1 Customizable M functions 13-2 M function Descriptions 13-3

CHAPTER 14 – Configuration

Password 14-1 Control Configuration 14-2 User Specified Paths 14-3 Machine Configuration 14-4 Machine Parameters 14-8 PID Menu 14-42 DSP Probe Configuration 14-45 Smoothing 14-47

CHAPTER 15 – CNC Software Messages

CNC Software Message Descriptions 15-1

Page 7

Page 8

Chapter 1

Introduction

Window Description

The CNC software display screen is separated into five areas called windows. A sample screen is shown below for reference. The five windows are the DRO display window, the status window, the message window, the options window, and the user window. The information that each window displays is described in detail in the following sections.

DRO display

The DRO display contains the digital read out of the current position of the tool. The display is configurable for number of axes and desired display units of measure (see Chapter 14). The bars under each axis are the load meters and represent the amount of power being supplied to the drive for that axis. The display of axis load meters is configured by machine parameter 143 – see Chapter 14 for specific information.

Distance to Go DRO

The distance to go DRO is located below the main DRO. This display shows the distance to go to complete the current movement. The display of distance to go is controlled by parameter 143. See Chapter 14 for details. See also “Hot Keys” in chapter 2.

M-Series Operator’s Manual 12/20/13 1-1

Page 9

Status window

The first line in the status window contains the name of the currently loaded job file. Below the job name are the Tool Number, Program Number, Feedrate Override, Spindle Speed, and Feed Hold indicators. The Feedrate Override indicator displays the current override percentage set on the Jog Panel. The Feedrate label will turn RED if the rapid override is turn off. If your machine is equipped with a variable frequency spindle drive (inverter), the Spindle indicator will display the current spindle speed. The Feed Hold indicator displays the current status (on/off) of FEED HOLD. See Chapter 2 for descriptions of the Feed Hold Button, Feedrate Override Knob, and Spindle controls. For a description of the Program Number see G65 in Chapter 12 or M98 in Chapter 13.

The Part Cnt and Elapsed Time indicators appear when CYCLE START is pressed while a job is running. The Part Count indicator displays the number of times the currently loaded job has been run. They count increments by one after the completion of a run. If a job is canceled prematurely, the part count will not be incremented. The Part # counter shows the how many parts have been run, with an up/down arrow displayed to indicate the counting direction. See the run menu for more information on the Part Cnt and Part # setting.

The Part Time indicator displays how much time has passed since the CYCLE START button was pressed. The indicator will help you to determine how long it takes to mill a particular part. The timer will not stop until the job is canceled. It will continue to count for optional stops, tool changes, FEED HOLD, etc.

Message window

The message window is divided into a message section and a prompt section. The prompt section of the window is the lowest text line in the window and will display prompts to the user. For example, the prompt 'Press CYCLE START to start job' is displayed on the prompt line after power-up.

The message section is the top four text lines of the message window. This section will display warnings, errors, or status messages. The newest messages always appear on the lowest of the four lines. Old messages are shifted up until they disappear off the top of the message window. When old messages scroll out of view, a scroll bar will appear on the right side of the window. When the scroll bar is visible you may use the up and down arrow keys to view older messages. See Chapter 15 for a description of the CNC software error and status messages.

Options window

Options are selected by pressing the function key indicated in the box. For example, on the main screen, pressing the function key F5 - CAM selects the CAM option.

User window

The information contained in this window is dependent upon on the operation the user is performing on the control. If no action is being taken, the window is empty.

For instance, when the CYCLE START button is pressed and a job is processed correctly, up to 11 lines of G codes will be displayed in this window for the user to observe during the Run of the part. All of the part zeros, the tool library setup, and the Digitizing/Probing information are entered in by the user in this window.

M-Series Operator’s Manual 12/20/13 1-2

Page 10

Conventions

*Bold capitalized characters represent keystrokes. For example, the A key is written as A, and the enter key is written as ENTER. The "Escape" key is written as ESC. Key combinations such as ALT- D mean that you should press and hold ALT then press D.

*All data entry screens in the M-Series Control use F10 to save changes.

*Any menu in the M-Series Control can be exited by pressing ESC. This will take you back to the previous menu. This also usually discards any changes you have made in that menu.

*All program examples and software use the standard Cartesian coordinate system (see the figure below). If you are facing the mill, the X-axis is defined positive to your right; the Y-axis is defined positive to the mill; and the Zaxis is defined positive upward, perpendicular to the XY plane.

*The direction of motion is defined by the CUTTER motion, not the TABLE motion.

*CW stands for clockwise, and CCW stands for counterclockwise.

M-Series Operator’s Manual 12/20/13 1-3

Page 11

Machine Home

When the M-Series control is first started, the Main screen will appear as below.

Before you can run any jobs, you must set the machine home position. If your machine has home/limit switches, reference marks or safe hard stops, the control can automatically home itself. If your machine has reference marks, jog the machine until the reference marks are lined up, (see below), before you press CYCLE START to begin the automatic homing sequence. The control will execute the G-codes in a file called cncm.hom in the c:\cncm directory. By default, this file contains commands to home Z in the plus direction, then X in the minus and Y in the plus direction.

Typical Reference Marks

If your machine does not have home/limit switches or safe hard stops, the following message will appear instead.

In this case you must move the machine to its home position yourself, using either the jog keys or the handwheels. Once all axes are at their home positions, press CYCLE START to set machine home.

M-Series Operator’s Manual 12/20/13 1-4

Page 12

Mill M and G Codes

This is a summary list of M and G codes. See Chapters 12 – 13 for more information.

M00 Stop for Operator M01 Optional Stop for Operator M02 Restart Program M03 Spindle On Clockwise M04 Spindle On Counterclockwise M05 Spindle Stop M06 Tool Change M07 Mist Coolant On M08 Flood Coolant On M09 Coolant Off M10 Clamp On M11 Clamp Off M25 Move to Z Home M26 Set Axis Home M30 Customizable M-code for End of Intercon Program M39 Air Drill M91 Move to Minus Home M92 Move to Plus Home M93 Release/Restore Motor Power M94,M95 Output On/Off M98 Call Subprogram M99 Return from Macro or Subprogram M100 Wait for PLC bit (Open, Off, Reset) M101 Wait for PLC bit (Closed, On, Set) M102 Restart Program M103 Programmed Action Timer M104 Cancel Programmed Action Timer M105 Move Minus to Switch M106 Move Plus to Switch M107 Output BCD (Binary Coded Decimal) Tool Number M108 Enable Override Controls M109 Disable Override Controls M115,M116,M125,M126 Protected Move Probing M120 Open data file (overwrite existing file) M121 Open data file (append to existing file) M122 Record local position(s) in data file M123 Record value and/or comment in data file M124 Record machine position(s) in data file M127 Record Date and Time in a data file M128 Move Axis by Encoder Counts M129 Record Current Job file path to data file M130 Run system command M200/M201 Stop for Operator, Prompt for Action M223 Write Formatted String to File M224 Prompt for Operator Input Using Formatted String M225 Display Formatted String for A Period of Time M300 Fast Synchronous I/O update M1000-M1015 Graphing Color for Feedrate movement

G00 - Rapid to Position G01 - Linear Move G02/G03 - CW/CCW Arc Move G04 - Dwell G09 - Decel and Stop G10 - Set Parameter G17/G18/G19 - XY/ZX/YZ Plane Selection G20 - Inch Units G21 - Metric Units G22 - Work Envelope On G23 - Work Envelope Off G28 - Return to Reference Point G29 - Return from Reference Point G30 - Return to Secondary Reference Point G40 - Cancel Cutter Compensation G41/G42 - Cutter Compensation Left/Right G43/G44 - Tool Length Compensation +/G49 - Cancel Tool Length Compensation G50 - Cancel Scaling / Mirroring G51 - Scaling / Mirroring G52 - Offset Local Coordinate System Origin G53 - Rapid Positioning in Machine Coordinates G54-G59 - Select Work Coordinate System G61 - Modal Decel and Stop G64 - Smoothing Mode Selection / Cancel Modal Decel and Stop G65 - Call Macro G68 - Rotate G69 - Cancel Rotate G73 - High Speed Peck Drilling (Canned Cycle) G74 - Counter Tapping (Canned Cycle) G76 - Fine Bore (Canned Cycle) G80 - Cancel Canned Cycle G81 - Drilling and Spot Drilling (Canned Cycle) G82 - Drill with dwell (Canned Cycle) G83 - Deep hole drilling (Canned Cycle) G84 - Tapping (Canned Cycle) G85 - Boring (Canned Cycle) G89 - Boring with dwell (Canned Cycle) G90 - Absolute Positioning Mode G91 - Incremental Positioning Mode G92 - Set Absolute Position G93 - Inverse Time Feedrate Mode G94 - Cancel Inverse Time Feedrate Mode G98 - Initial Point Return G99 - R Point Return G117/G118/G119 - XY/ZX/YZ Plane Selection & Rotation G173,G174,G176,G181,G182,G183,G184,G185,G189

- Compound Canned Cycles G180 - Cancel Canned Cycle

M-Series Operator’s Manual 12/20/13 1-5

Page 13

How to unlock software features or unlock your Control

The following are necessary to unlock software features:

1. If you are at the "Demo mode expired" screen, start at step 4.

2. Go to the Main screen of the Control software.

3. Press F7 "Utility" and then F8 "Option"

4. Press F1 "Unlock Option". (You may need to enter the password – usually 137)

5. Next, type in the Unlock # and press ENTER.

6. Then, type in the Unlock Value and press ENTER.

7. Repeat step 4, 5, and 6 for each new Unlock.

M-Series Operator’s Manual 12/20/13 1-6

Page 14

Chapter 2

Operator Panel

The M-Series operator panel is a sealed membrane keyboard that enables you to control various machine operations and functions. The panel contains momentary membrane switches. The M-Series jog panel can be customized as to the location of various keys. The jog panel displayed in the figure above is representative of a default configuration found on most M-series controls.

Axis Jog Buttons

X+ X- Y+ Y- Z+ Z- 4TH+ 4TH-

The yellow X, Y, Z, and 4TH keys are momentary switches for jogging each of the four axes of the machine. There are two buttons for each axis (+/-). Only one axis can be jogged at a time.

* NOTE: The jog buttons will not operate if the M-Series CNC software is not running, or if a job (a CNC program) is running.

Slow/Fast

The slow/fast key is located in the center of the Axis Motion Controls section and is labeled with the turtle and rabbit icon shown to the right. The turtle represents slow jogging mode. When SLOW jog is selected (LED on) and a jog button is pressed, the axis moves at the slow jog rate. If FAST jog is selected, the axis will move at the fast jog rate. See Chapter 14 for information on setting the fast and slow jog rates for each axis.

Inc/Cont

INC/CONT selects between incremental and continuous

jogging. Pressing the key will toggle between these two

Fig 1 - M-Series Jog Panel

modes. The LED is lit when INC is selected. If CONT jog is selected and an axis jog button is pressed, the axis will move continuously until the button is released.

x1, x10, x100

Press any one of these keys to set the jog increment amount. The amount you select is the distance the control will move an axis if you make an incremental jog (x1=0.0001", x10=0.0010" and x100=0.0100"). You may select only one jog increment at a time, and the current jog increment is indicated by the key that has a lit LED. The jog increment you select is for all axes; you cannot set separate jog increments for each axis. The jog increment also selects the distance the control will move an axis for each click of the MPG handwheel.

M-Series Operator’s Manual 12/20/13 2-1

Page 15

MPG

The MPG is housed in a separate hand-held unit. Press the MPG key to set the control jog to respond to the MPG hand wheel, if equipped. When selected, the LED will be on. Select the Jog Increment and desired axis and slowly turn the wheel. When the LED is not lit, the MPG is disabled and the jog panel is on.

Single Block

The SINGLE BLOCK key selects between auto and single block mode. When the SINGLE BLOCK LED is on, the single block mode has been enabled. Single Block mode allows you to run a program line by line by pressing CYCLE START after each block. While in block mode you can select auto mode at any time. While in auto mode and a program is running you cannot select single block mode. Auto mode runs the loaded program after CYCLE START is pressed. Auto mode is the default (LED off).

Cycle Start

When the CYCLE START button is pressed, the M-400/M-39 Control will immediately begin processing the current program at the beginning and will prompt you to press the CYCLE START button again to begin execution of the program. After an M0, M1, M2, or M6 is encountered in the program, the message “Press CYCLE START to continue” will be displayed on the screen, and the M-400/M-39 Control will wait until you press the CYCLE START button before continuing program execution.

WARNING

Pressing CYCLE START will cause the M-Series Control to start moving the axes immediately without further warning. Be certain that you are ready to start the program when you press this button. Pressing the FEED HOLD button or the CYCLE CANCEL button will stop any movement if CYCLE START is pressed accidentally.

Feedrate Override

This knob controls the percentage of the programmed Feedrate that you can use during feedrate cutting moves: lines, arcs, canned cycles, etc. This percentage can be from 0% to 200%.

CAUTION

The Feerate Override knob will not work during tapping cycles (G74 and G84).

Feed Hold

Feed Hold decelerates motion of the current movement to a stop, pausing the job that is currently running. Pressing CYCLE START will continue the movement from the stopped location.

CAUTION

FEED HOLD is temporarily disabled during tapping cycles (G74 and G84) and automatic tool changes (M6).

Tool Check

Press TOOL CHECK while no program is running to move the Z-axis to its home position/G28 position. Press TOOL CHECK while a program is running to abort the currently running program. The control will stop normal

program movement, pull Z to its home position, clear all M-functions, and automatically display the Resume Job Screen. From the Resume Job Screen, you can change tool settings (height offsets, diameter offsets, etc.) and resume the job with the new tool settings.

M-Series Operator’s Manual 12/20/13 2-2

Page 16

Cycle Cancel

Press CYCLE CANCEL to abort the currently running program. The control will stop movement immediately, clear all M-functions, and return to the Main Screen. It is recommended that you press FEED HOLD first before CYCLE CANCEL. If you press CYCLE CANCEL, program execution will stop; if you wish to restart the program you must rerun the entire program or use the search function. See search function operation in Chapter 3 or Chapter 6.

Emergency Stop

EMERGENCY STOP releases the power to all the axes and cancels the current job immediately upon being pressed. EMERGENCY STOP also resets certain faults if the fault condition has been fixed or cleared.

WARNING

On some machines, vertical axes (such as Z and/or W) may start to move due to gravity pulling it down when motor power is cut due to EMERGENCY STOP being pressed.

Spindle CW/CCW

The SPINDLE CLOCKWISE/COUNTERCLOCKWISE keys determine the direction the spindle will turn if it is started manually. If the spindle is started automatically, the direction keys are ignored and the spindle runs according to the program. The default direction is CW.

Spindle Speed +

Pressing this key will increase the spindle speed by 10% of the commanded speed in Auto spindle mode, limited by the maximum speed or 200% of commanded speed, whichever is less. For manual spindle mode, the spindle speed is increased by 5% of the maximum spindle speed (up to the maximum speed). The LED is on if the spindle speed is set above the 100% point.

Spindle Speed 100%

Pressing this key will set the spindle speed at the 100% point, which is defined as the commanded speed in Auto spindle mode, or ½ the maximum spindle speed in manual mode. The LED will be on when the spindle is at the 100% point.

Spindle Speed -

Pressing this key will decrease the spindle speed by 10% of the commanded speed in Auto spindle mode, limited to 10% of commanded speed. For manual spindle mode, the spindle speed is decreased by 5% of the maximum spindle speed down to 5% of maximum. The LED is on if the spindle speed is set below the 100% point.

Spindle (Auto/Man)

This key selects whether the spindle will operate under program control (automatic) or under operator control (manual). When the LED is lit, the spindle is under automatic control. If the LED is off, the spindle is under manual control. Pressing the SPINDLE (AUTO/MAN) key will toggle it from AUTO to MAN and back again. The default is AUTO mode.

M-Series Operator’s Manual 12/20/13 2-3

Page 17

Spin Start

Press the SPIN START key when manual spindle mode is selected to cause the spindle to start rotating. Press SPIN START when automatic mode is selected to restart the spindle if it has been paused with SPIN STOP.

Spin Stop

Press the SPIN STOP key when manual spindle mode is selected to stop the spindle. Press SPIN STOP when automatic mode is selected to pause spindle rotation and can be restarted with SPIN START.

NOTICE

SPIN STOP should only be pressed during FEED HOLD or when a program is NOT running.

Coolant Auto/Manual

This key will toggle between automatic and manual control of coolant. In automatic mode, M7 (Mist) and M8 (Flood) can be used in G-code programs to select the coolant type to be enabled. In manual mode, flood coolant and mist coolant are controlled by separate keys. Note: When switching from automatic to manual mode, both flood and mist coolants are turned off automatically.

Coolant Flood

In manual coolant control mode, flood coolant can be toggled off and on by pressing this key. The LED will be on when flood control is selected in either automatic or manual mode.

Coolant Mist

In manual coolant control mode, mist coolant can be toggled off and on by pressing this key. The LED will be on when mist control is selected in either automatic or manual mode.

Auxiliary Function Keys (AUX1 – AUX12)

The M-Series jog panel has nine auxiliary keys, some of which may be defined by customized systems.

Notes about operator panels

The behavior of the control system in response to the functions listed above for the M-Series jog panel is dependent upon optional software options, the PLC program, machine parameters, and hardware wiring of the system. It is possible that the functioning explained in this chapter does not apply to a particular control system or that it may differ in some aspects.

M-Series Operator’s Manual 12/20/13 2-4

Page 18

Keyboard Jog Panel

The PC keyboard may be used as a jog panel. Press Alt-J to display and enable the keyboard jog panel. The jog panel appears as shown below:

Some controls, such as coolant on/off, spindle on/off, feedrate and spindle override will work without the “jog panel” being displayed but for full functionality (and jogging) of the keyboard jog panel, the “jog panel” must be displayed on the screen. To enable keyboard jogging, parameter 170 must be set to “1”.

The status window in the upper right corner of the screen displays the jogging mode (continuous/incremental), incremental step size, and jog speed (fast/slow). In continuous mode, the jog keys start movement when pressed and movement stops when you release the key. In incremental mode, the axis will move the indicated incremental step amount.

As shown in the picture above, the jog keys are located in the cursor key block to the right of the main keyboard and to the left of the numeric keypad. If a jog key controls an axis, it will be overlaid with the axis symbol (“X”, “Y”, etc.) The jog keys are the arrow keys, Page Up, and Page Down.

The remaining keys are described below:

Legend Key(s) Function Description Availability (Notes)

Ctrl S Cycle Start Same as Cycle Start. Always, with few

Esc Cycle

Space

Cancel

Feed Hold Turns Feed Hold on and off Always, with few

Same as Cycle Cancel. During a job run;

exceptions.

otherwise, Esc is used to exit menus.

exceptions.

Alt J Start/Exit

Panel

Ctrl F1

Ctrl F12

M-Series Operator’s Manual 12/20/13 2-5

Aux 1 – Aux 12

Invokes or exits the jog panel. Always, with few

exceptions. Executes the corresponding Aux function and signals the PLC. A custom PLC program is required to act upon jog panel signals.

Always, with few

exceptions.

Page 19

Legend Key(s) Function Description Availability (Notes)

Feedrate Override +

Ctrl M Toggle Auto

Coolant

Ctrl N Turns on/off

Flood

Ctrl K Turns on/off

Mist

Ctrl +

Increase feedrate override

Toggles coolant mode between auto and manual.

Toggles Flood coolant if in manual mode Always, with few

Toggles Mist coolant if in manual mode Always, with few

Increase feed rate override by 1% while held. Jog panel, job run,

Always, with few exceptions.

exceptions.

graphing, and some other times

Feedrate Override

Ctrl -

Ctrl C Selects CW

Ctrl W Selects CW

Decrease feedrate override

Spin

Decrease feed rate override by 1% while held. Jog panel, job run,

graphing, and some other times.

Selects CW Spin dir in man mode Always, with few

exceptions.

Selects CCW Spin dir in man mode Always, with few

exceptions.

Ctrl A

Ctrl S Spin Start Starts spindle in selected direction if in

Ctrl Q

Ctrl > Spindle

Ctrl < Spindle

Ctrl T

Ctrl I Incremental/

Ctrl B Selects

M-Series Operator’s Manual 12/20/13 2-6

Toggle Spindle Auto/ Manual

Spin Stop STOPS spindle regardless of auto or manual

Override +1%

Override 1%

Tool Check Performs a tool check.

Continuous Jog Selection

Single Block Mode

Toggles between automatic and manual spindle operation.

manual mode

mode.

Increase the spindle override by 1% while held.

Decrease the spindle override by 1% while held.

Toggles incremental or continuous jog mode. Available most times

Selects single block mode Always, with few

Always, with few exceptions.

that jogging is available.

exceptions.

Page 20

Legend Key(s) Function Description Availability (Notes)

Delete Decrease

Jog

Insert Increase Jog

Left arrow

Right Arrow

Up Arrow

Down Arrow

Page Up Z + Jog With on screen jog

increment

Increment

X - Jog With on screen jog

X+ Jog With on screen jog

Y+ Jog With on screen jog

Y- Jog With on screen jog

Decreases current jog increment to the next lower available increment

Increase current jog increment to the next higher available increment

Always, with few

exceptions.

Always, with few

exceptions.

panel displayed

Page Down

Z - Jog With on screen jog

panel displayed

MDI and the Keyboard Jog Panel

Many of the keys used by the keyboard jog panel are also possible commands to MDI. To use the keyboard jog panel functions in MDI, you must press Alt J. You may jog; use the handwheels, or any other jog panel function. Press Alt

J or Esc to return to MDI.

Keyboard Shortcut Keys

A computer style keyboard is supplied with most systems. This keyboard can be used as a jog panel. The keyboard jog panel has many “hot keys”. Hot keys are keys that can be used at almost any time, with few exceptions. Some menus may prohibit their use. The CNC software has many other hot keys in addition to the jog panel hot keys. The hot keys are listed below.

Hot Keys

Hot Key Action

Ctrl A Spindle auto/manual Ctrl N Flood coolant on/off* Ctrl M Toggle Auto Man Coolant ALT D Switch between current position and machine position CTRL D Switch DRO between position and distance to go CTRL K Mist coolant on/off* ALT F Displays available system memory ALT I PLC diagnostics

M-Series Operator’s Manual 12/20/13 2-7

Page 21

Hot Key Action

ALT J Enables keyboard jogging* ALT K Displays current ATC tool bin location ALT M MDI Ctrl T Tool check* ALT P Live PID display CTRL P Clear max and min error display Ctrl C Spindle CW* Ctrl W Spindle CCW* Ctrl S Start Spindle* Ctrl Q Stop Spindle ALT S Cycle start ALT T Displays current motor temperature estimates ALT V Displays current software version # ALT W MPG on/off* ALT + / ALT - Selects next/previous WCS, cycles through WCS 1-18** ALT 1 - ALT 0 Selects WCS 1 – WCS 10** ALT Tab Cycle through currently running applications CTRL F1 - CTRL F12 Executes Aux function 1 – 12* CTRL V Enables/disables Stall detection in PID Configuration*** CTRL I Creates plcstate.txt when PLC diagnostics is displayed*** CTRL E Starts the PLC Debugger***

Notes: * This is a keyboard jog panel function.

** Not available during jobs or on jog panel.

M-Series Operator’s Manual 12/20/13 2-8

Page 22

Chapter 3

CNC Software Main Screen

Menu Options:

F1 – Setup Used to set part zeroes, set or change tool offsets, and change the control configuration. F2 – Load Use this menu to load a job F3 – MDI The MDI menu allows you to a single line command such as: G1 X2 Y3 F20

F4 – Run Use the Run menu to search and run a job from a specific line, resume a job after it has

been canceled or to change the way a job runs.

F5 – CAM Use the CAM menu to program parts. F6 – Edit Brings up a G-code (text) editor that allows you to edit the currently loaded job. F7 – Utility View available software options, backup part and configuration files, create new

directories, and import/export files to and from external locations.

F8 – Graph Graphs the toolpath of the currently loaded part program.

F9 – Digitize Displayed only if the Digitizing option has been purchased. Used to Digitize (reverse

engineer) parts.

F10 – Shut down Power off control. Shutting down your machine without using this menu may damage

your control.

M-Series Operator’s Manual

12/20/13

3-1

Page 23

F1- Setup Menu

Setup Menu: F1 – Part This key displays the Part Setup menus that are explained in Chapter 4. F2 – Tool This key displays the Tool Setup menus that are explained in Chapter 5. F3 – Config This key displays the Configuration menu that is explained in Chapter 14. F4 – Feed This key displays the Feed menu that is discussed in Chapter 6. F5 – 3rd Axis Toggle This key will only be displayed if machine parameter 130 is set. See Chapter 14

for configuration options.

F6 – 4th Axis Toggle This key will only be displayed if machine parameter 131 is set. See Chapter 14

for configuration options.

F7 – ATC This key will only be displayed if machine parameter 6 is set to 1.0. It has the

same effect as the F7 - ATC key in the Tool menus. It will prompt you for a tool number and then perform the actions required for an automatic tool change cycle.

F8 – Smoothing Setup This gives you acces to the Smoothing Setup Menu which provides a simplified

way of choosing parameters for the Smoothing module. See Chapter 14 under “Smoothing Setup Menu”.

M-Series Operator’s Manual

12/20/13

3-2

Page 24

F2- Load Job Menu

Floppy

Floppy Floppy

Floppy

FFFF

2222

Details

DetailsDetails

Details

FFFF

3333

Show

ShowShow

Show

FFFF

4444

Date/

Date/Date/

Date/

FFFF

5555

FFFF

6666

Help

HelpHelp

Help

FFFF

7777

FFFF

9999

F1F1

0000

G code

G code G code

G code

F1F1

Job Name: c:

cnc

m\ncfiles

bracket.cnc

Use arrow keys to select file to load and press F10 to Accept.

Use arrow keys to select file to load and press F10 to Accept.Use arrow keys to select file to load and press F10 to Accept.

Use arrow keys to select file to load and press F10 to Accept.

////USB/LAN

USB/LAN

USB/LANUSB/LAN

Edit

On/Off

On/OffOn/Off

Recent

RecentRecent

Alpha

AlphaAlpha

EditEdit

On////Off

Off

OnOn

OffOff

Graph

Graph Graph

Advanced

AdvancedAdvanced

AcceptAccept

arcs.cnc

arcs.cncarcs.cnc bracket.cnc

bracket.cnc

bracket.cncbracket.cnc flange.cnc

flange.cnc

flange.cncflange.cnc test fixture plate.cnc

test fixture plate.cnc

test fixture plate.cnctest fixture plate.cnc

Job

Job to

to load? bracket.cnc

load? bracket.cnc

Job Job

toto

load? bracket.cnc load? bracket.cnc

/ICN

/ICN/ICN

F1 – G code/ICN Allows the user to change which types of files are displayed.

F2 – Floppy/USB/LAN Select a different drive from which to load files.

F3 – Details Displays file details including: Programmer, Description and Date Modified. F4 – Show Recent Displays a list of the 15 most recently loaded jobs.

F5 – Date/Alpha Toggles the current view of files to be sorted alphabetically or by date modified. F6 – Edit Opens selected file in editor. F7 - Help Displays on screen help for the load screen. F8 - Graph Backplots (graphs) the selected file. F9 - Advanced Displays a unified file and device browser similar to Windows Explorer.

Page Up Move the cursor backward one page. Page Down Move the cursor forward one page. END Select the last file in the list. HOME Select the first file in the list. Arrow Keys

*Note: The path and/or file name may also be selected by typing the path or path and file name. A window

will open automatically when you begin typing.

M-Series Operator’s Manual

12/20/13

3-3

Page 25

F3 –MDI

Pres

PresPres

Pres

s CYCLE START to start job

s CYCLE START to start jobs CYCLE START to start job

s CYCLE START to start job

Repeat

Repeat Repeat

Repeat

F3F3

/Skips

/Skips /Skips

/Skips

Off

Off Off

Off

F F

4444

RTG

RTG RTG

RTG

Rapid

Rapid Rapid

Rapid

Single Block Mode:

Single Block Mode:Single Block Mode:

Single Block Mode:

Off

OffOff

Off

Run

RunRun

Run

RunRun

Run

----

Time Graphics:

Time Graphics:Time Graphics:

Time Graphics:

Off

OffOff

Off

MDI mode allows you to directly enter M and G-codes one line at time. After entering the M and Gcodes you wish to run, press cycle start to have the controller execute the command. When the command has finished executing the command, it will prompt you for another line. When you are finished entering commands, press ESC.

Examples:

Block? G92X0Y0 ; Set the current XY position to 0,0 Block? M92 /Z ; Move the Z to the positive limit. Block? M26 /Z ; Set the current Z position as Z home

F4 – Run Menu

X +4.0000

X +4.0000X +4.0000 Y +2.0000

Y +2.0000

Y +2.0000Y +2.0000 ZZZZ

----

Optional Stops:

Optional Stops: Off

Optional Stops:Optional Stops:

Block Skips:

Block Skips: On

Block Skips:Block Skips:

Job Repeat:

Job Repeat: Off

Job Repeat:Job Repeat:

Run job options:

F2 – Search You can resume a job by searching for the line, tool, or a block number. F3 – Repeat Toggles Job Repeat. Will repeat the current program when a job is finished. F4 – Block Skips Turns on and off block skips in part programs. F5 – Single Block Program runs in single block mode when turned on. F6 – Stops Turns on and off optional stops (M01) in part programs. F8 – Graph Graphs tool path of currently loaded program F9 – Rapid Turns on and off rapid override function F10 – RTG Turns on and off Run Time Graphics

*Note: For more information on these options, please see chapter 6.

Current Position (

Current Position ( Inches

Current Position (Current Position (

Search Search

On On

Inches )

)

InchesInches

0.5000

0.50000.5000

Off

OffOff

OnOn

Off

OffOff

) )

Block

BlockBlock

Stops

Stops Stops

Job Name :

Job Name : bbbbracket.cnc

Job Name : Job Name : Tool :

Tool : T001 H001

Tool : Tool : Feedrate : 100%

Feedrate : 100%

Feedrate : 100%Feedrate : 100% Sp

Spindle : 0 M

indle : 0 M

SpSp

indle : 0 M indle : 0 M

Stopped

StoppedStopped Waiting for PLC operation

Waiting for PLC operation

Waiting for PLC operationWaiting for PLC operation

racket.cnc

racket.cncracket.cnc

T001 H001

T001 H001T001 H001

Graph

GraphGraph

Off

Off Off F9

F9 F9

On/Off

On/OffOn/Off

M-Series Operator’s Manual

12/20/13

3-4

Page 26

F5 – CAM

ICN

ICNICN

ICN

----

Intercon Mill

Intercon Mill Intercon Mill

Intercon Mill

CAM Selection

CAM SelectionCAM Selection

CAM Selection

Waiting for PLC operation

Waiting for PLC operationWaiting for PLC operation

Waiting for PLC operation

Pres

PresPres

Pres

s CYCLE START t

s CYCLE START ts CYCLE START t

s CYCLE START t

o start job

o start jobo start job

o start job

ICN

ICNICN

ICN

----

Intercon Mill

Intercon Mill Intercon Mill

Intercon Mill

X +4.0000

X +4.0000X +4.0000

Y +2.0000

Y +2.0000Y +2.0000

ZZZZ

----

Current Position (

Current Position ( Inches

Current Position (Current Position (

0.5000

0.50000.5000

Inches )

InchesInches

)

) )

Job

Job Name :

Job Job Tool :

Tool : T001 H001

Tool : Tool : Feedrate : 100%

Feedrate : 100%

Feedrate : 100%Feedrate : 100% Spindle : 0 M

Spindle : 0 M

Spindle : 0 M Spindle : 0 M

Stopped

StoppedStopped

: bbbbracket.cnc

racket.cnc

: :

racket.cncracket.cnc

T001 H001

T001 H001T001 H001

CAM

CAM Selection

Selection

CAMCAM

Selection Selection

Engrave

Engrave ---- DXF Engraving

EngraveEngrave

Milwrt

Milwrt ---- Millwrite Engraving

Milwrt Milwrt

Manual

ManualManual

---- Operators Manual

DXF Engraving

DXF Engraving DXF Engraving

Engrave

EngraveEngrave

Milwrt

MilwrtMilwrt

Help

HelpHelp

---- DXF Engraving

DXF Engraving

Millwrite Engraving

Millwrite Engraving Millwrite Engraving Operators Manual

Operators Manual Operators Manual

DXF EngravingDXF Engraving

---- Millwrite Engraving

Millwrite Engraving

Millwrite Engraving Millwrite Engraving

---- Operators Manual

Operators Manual

Operators Manual Operators Manual

ICN

ICNICN

Engrave

EngraveEngrave

Milwrt

MilwrtMilwrt

Manual

ManualManual

Choose F5-CAM to program parts. The default part programming system is Intercon. Intercon is a

conversational programming system that allows you to quickly and easily create a part program. Intercon features many easy to use canned cycles for most common machining operations such as: rectangular, circular and irregular pockets, pockets with islands, bolt hole circles, frames, thread milling operations and much more. When you are finished programming your part in Intercon, exit to return to the M-Series Control Main Screen and the posted Intercon program will be automatically loaded and ready to run. For more information on Intercon, see chapter 10.

F1 – ICN Intercon conversational program system F2 – Engrave DXF engrave option (optional item part of DXF Import) allows you to import an entire DXF

drawing and engrave it onto a part.

F3 – Milwrite Millwrite Engraving software (optional item) allows you to create engraving files to engrave

letters, numbers, and symbols on your parts.

F4 – Manual Allows you to access the operator manual on the control

M-Series Operator’s Manual

12/20/13

3-5

Page 27

F6 – Edit

This key causes the control to load the current job into a text editor for viewing and/or editing. When editing, care must be taken to save the file and to quit and exit the text editor before running the file

(the current job). Modifying a file that is currently running as the current job is dangerous and will cause unexpected results. It is best practice to not edit any files while the machine is moving.

WARNING

Also, note that the C:\CNCM directory contains configuration files and binary data. DO NOT edit these files. Doing so can cause loss of data and serious malfunctions.

WARNING

Editing a file (modifying and saving) while the machine is moving can cause personal injury or machine damage.

Do not edit configuration data located in the C:\CNCM directory. Doing so can cause personal injury or machine damage.

F7 – Utility

From the utility menu you can view available software options, perform diagnostics, backup part and configuration files, create new directories and import or export files to and from external locations. For

further information please see chapter 7. F2 – Restore Report Update your control’s configuration with a report.zip file.

F3 – Backup Files Backup your CNC and ICN files F4 – Restore Files Restore your CNC and ICN files F5 – File Ops Use this menu to perform file and directory operations. F6 – User Maint Perform user maintenance. F7 – Create Report Generates a backup of system configuration files called report.zip. F8 – Options Shows the software options that you have purchased or added to your control. F9 – Logs Shows the messages and errors that have been logged by the control.

M-Series Operator’s Manual

12/20/13

3-6

Page 28

F8 – Graph

This function plots the tool path of the current program loaded. Canned drilling cycles are shown in gray. Rapid traverse movements are shown in red. Feedrate movements are shown in yellow and cutter compensated moves are in gray.

F1 - 2D/3D Press this key to view your part isometrically (3D). An axis pointer indicates the current

direction of the view. To return back to the tri-planar view, press F1 again.

F2 – View/Rotate Press this key to change the planar view of your part. The view is indicated by TOP,

RIGHT, or FRONT shown at the top of the screen. In 3D Mode, use this key in 3D mode to rotate your part, using the keyboard arrow keys to rotate any in direction.

F3 – Range Press this key to set the range of line numbers or block numbers to graph. F4 – Time Press this key to estimate the time needed to create part. It takes into account

accelerations and decelerations, but neglects tool change times.

F5 – Redraw Press this key to redraw the part at any time. F6 – Pan Press this key to move the part around the screen. Once pressed, use the crosshairs to

pick a location of the part that will redraw at the center of the screen. Once a section is selected, press F6 again to continue panning.

F7 - Zoom In Press these keys to zoom into the part relative to the center of the screen. F8 - Zoom Out Press these keys to zoom away from the part relative to the center of the screen. F9 - Zoom All Press this key to view the entire part fit inside the screen.

*Note: Use the FEEDRATE OVERRIDE knob to control the speed of the graphing. To pause the tool path,

turn the knob counter-clockwise until it stops. Turn the knob clockwise to resume drawing. On the offline demo software, the simulated FEEDRATE OVERRIDE knob is controlled by pressing either Ctrl + or Ctrl –.

M-Series Operator’s Manual

12/20/13

3-7

Page 29

Accelerated Graphics Backplot

Accelerated Graphics Backplot is a new tool path graphics display that takes advantage of the latest video graphics technology. This option is enabled by setting Parameter 260 to 1 (See Chapter 14). Under Accelerated Graphics Backplot, the operation of the user interface is slightly different from the regular Graphing described above.

F1 - Pan/Rotate Press this key to change the behavior of the keyboard arrow keys. Normally, they will

pan (scroll) around the drawing, but after pressing this key the arrow keys will control rotation instead. When in rotation mode, an axis indicator is drawn to mark the center of rotation.

F2 - View Press this key to change the planar view of your part. The view is indicated by TOP,

RIGHT, or FRONT shown at the top of the screen.

F3 - Set Range Press this key to select which lines of G-code to display. Only lines that fall within

the range you specify will be drawn.

M-Series Operator’s Manual

12/20/13

3-8

Page 30

F4 - Dimension Menu Press this key to access the following sub-menu of options:

F1 – Prev Line: Press this to walk forward to the next G-code line and graphically

highlight it. If this G-code line contains movement, the Start and End points will be displayed at the bottom of the screen. F2 – Next Line: Press this to walk backward to the previous G-code line and graphically highlight it. If this G-code line contains movement, the Start and End points will be displayed at the bottom of the screen. F3 – Go To Line: Press this key to graphically highlight a particular G-code line whose line number you specify. If this G-code line contains movement, the Start and End points will be displayed. F4 – Measure: Use this feature to measure between any 2 selected points. To do this, use a mouse to move the pointer over the first point and then press F4 – Measure to anchor the first point. Then use the mouse to move the pointer to the second point. As you move the mouse towards the second point, you will notice an Offset and Measurement display changing dynamically as you move the mouse. Also you may notice some “snap to” effects as you move the pointer close to start and end points of entities that make up your program.

F5 - Redraw Press this key to redraw the part slowly, which can be useful for visualizing the

movements the machine will make. While the display is being redrawn, you can use the feedrate override knob to adjust the rate at which it is being drawn. If you don't have a feedrate override knob, the + and - keys can be used to adjust the rate. Pressing F5 again will cancel this mode.

F6 - Hide Rapids Press this key to hide rapid movements. Press it again to show them. F7 - Zoom In Press these keys to zoom into the part relative to the center of the screen. F8 - Zoom Out Press these keys to zoom away from the part relative to the center of the screen. F9 - Zoom All Press this key to fit the entire part inside the screen. F10 - Show Tools Press this key to show the tools menu, which allows you to highlight movements of

certain tools. Press this key again to hide the tools menu.

Spacebar - Measure Press this key to take a measurement between two points. In a 2D view, this

measurement will be a 2D measurement. In a 3D view, it will be a 3D measurement (and the measurement will only be valid if the crosshairs are snapped to a line of the tool path).

*Note: If you have a mouse or touch screen attached to your device, you can use that to control the graphing window. Holding the left mouse button allows you to drag the part across the screen, while the right mouse button controls rotation of the part. Spinning the mouse wheel (or holding both left and right buttons) zooms in and out. Double clicking on a feedrate movement will center the camera on that movement (which is very useful) and also tells you the length of that movement. For touchscreen operation, use the F1 key to switch between Pan and Rotate modes.

M-Series Operator’s Manual

12/20/13

3-9

Page 31

F9 – Digitize

Use this to bring up the Digitize screen. This screen allows you to set up and run touch probe digitizing. See Chapter 8 for a detailed description of the digitizing operation.

F10 – Shutdown

Use to enter the Shutdown menu. This menu allows you to park the machine, power off the control, start a command window or exit CNC software.

F1 – Park Use this to park the machine at the end of the day for quicker machine homing at

startup. Once F10- Park is selected, The CYCLE START key must be press to start machine movement. The park feature homes each axis, at the maximum rate, to ¼ of a motor revolution from its home position.

F2 – Poweroff Use this to properly shutdown the control. With most controls, this action turns off

the control once the system has prepared itself to be shutdown. Just like a desktop computer, the control should be properly shutdown before turning off the power in order to reduce the risk of corrupting data on the hard drive. This will only turn off the control. The machine itself will still need to be manually turned off.

F6 – System Prompt This brings up the command line interface. Type the command exit to exit the

command window.

F9 – Exit CNC11 Use this to exit the CNC control software.

M-Series Operator’s Manual

12/20/13

3-10

Page 32

Chapter 4

Part Setup

(F1 from Setup)

The Part Setup menu is used to set the part position or the coordinate system origin for the part.

F1 – Next Axis Will toggle to the next axis. If changes were made to the current axis, but not yet accepted, they

will be discarded.

F4 – Auto Uses probe to automatically measure and set part position. Make sure your probe height and diameter

offsets are set for the tool number you assigned to the probe and that parameter 12 is set to that tool number. See Chapter 9 for more details.

F5 – Probe Will open the probing operations menu. See Chapter 9 for details.

F6 – Prev WCS Will select the previous work coordinate. The position being set will only affect the currently

selected work coordinate.

F7 – Next WCS: will select the next work coordinate. The position being set will only affect the currently selected

work coordinate.

F8 – CSR Will open the CSR menu, which can be used to automatically detect coordinate system rotation. This

function key appears only when the software option for Coordinate System Rotation is unlocked.

F9 – WCS Table Will open the Work Coordinate System (WCS) Configuration screen. See the Work Coordinate

System Configuration section later in this chapter for a complete description.

F10 – Set Will accept the position for the current axis, correcting for edge finder diameter based on the approach

direction if appropriate. It will not automatically advance to the next axis.

M-Series Operator’s Manual 12/20/13 4-1

Page 33

Operation Description

Z 0.0000

Setting the part position establishes a coordinate system with an origin at the part zero.

The F1 - Next Axis option selects the axis to be defined next. This field toggles between axis X, Y, Z, 4th, and 5th Axes. For each axis you will see a graphic description of the parameters to be entered, as well as the corresponding fields.

Setting up X or Y AXIS

Set Part Position

1) Select Axis with F1

2) Jog to Touch Off on Part

3) Edit the Value if Necessary

4) Press F10 to Set Position

Axis Part Edge Finder Approach Position Diameter from

X 0.0000 0.0000 Left (-)

Part Position: enter the value of your part zero position or the offset.

Edge Finder Diameter: enter the diameter of the tool, or edge finder you are using to determine the part zero. The value entered is stored.

Approach From: Toggle the direction the edge finder or probe is approaching the part.

*Note – Use the arrow keys to toggle between Part Position, Edge Finder Diameter, and Approach From options.

Setting up the Z AXIS

Set Part Position

1) Select Axis with F1

2) Jog to Touch Off on Part

3) Edit the Value if Necessary

4) Press F10 to Set Position

Axis Part Tool Position Number

Part Position: enter the value of your part zero position or the offset.

Tool Number: enter the tool number from the Tool Library that corresponds to the tool being used. When the Tool Number field is set to a value other than zero, the controller uses the Height Offset for that tool from the Tool Library to calculate the actual position.

M-Series Operator’s Manual 12/20/13 4-2

Page 34

Example 1 (You are using the reference tool to find the Z-axis part zero):

Set Tool Number to 0: setting the Tool Number to zero tells the controller that you are using the reference tool.

Example 2 (You are using a tool other than the reference tool, and not a ball nose cutter):

Set Tool Number to a number tool that is assigned in the tool library (make sure its height offset is set).

Example 3 (You are using a ball nose cutter, other than the reference tool):

Set Part Position to the position of the surface plus the nose radius of the ball nose cutter, set Tool Number to the number this tool is assigned in the tool library.

The Tool and Offset libraries must be up to date before setting the Z-axis Part Zero.

Setting up the 4th or 5th AXIS***

Position: enter the value of your part zero position or the offset.

Standoff Distance: this field is a generic parameter. Its physical meaning will depend on the specific nature of your machine's fourth axis. It is the distance between the center of the tool and the point at which the tool is touching the part surface.

Approach from: enter the direction the edge finder is approaching the part from. Enter the correct direction given the nature of your 4th-Axis.

Using Multiple Work Coordinate Systems

If you will be using multiple work coordinates, you must set the part position separately for each work coordinate. Follow the instructions above to set the position for each axis in the first coordinate system. Then move to the next fixture and press F6 – Prev WCS to select the previous work coordinate or F7 – Next WCS to select the next work coordinate. The currently selected coordinate system is displayed below the axis picture on the Part Setup screen. It is also displayed above the DRO at all times. For a description on setting up each work coordinate, see the Work Coordinate System Configuration section later in this chapter.

NOTICE

This procedure does NOT apply to tilt table setup.

M-Series Operator’s Manual 12/20/13 4-3

Page 35

Part Setup Examples

Example 1: Setting the X-axis Part Zero with no offset (See diagram below)

If you wanted the left edge of the part to be the origin for the X-axis:

1. Move the Edge Finder to the left edge of the part

2. Press F1 – Next Axis until the Axis label displays 'X'

3. Move the cursor to the Edge Finder Diameter field

4. Type .25 and press ENTER

5. Press SPACE until Left (-) is displayed

6. Press F10 - Set to accept the values

Axis Part Edge Finder Approach Position Diameter From X 0 0.25 Left (-)

Since no offset is being applied, Position is zero. The Edge Finder is approaching the part from the -X direction and has a diameter of .25 inches. Once this data is entered and F10 - Set is pressed, the X-axis DRO display will read -0.125. This means the center of the Edge Finder is sitting to the left (minus) of the part by 0.125 inches (half of the Edge Finder Diameter).

This value is computed by: Position (Approach from) Edge Finder Diameter / 2.

Where (Approach from) is the sign of the approach direction. In other words, if the approach direction is minus, then the value is: Position - Edge Finder Diameter / 2 = 0.0 - .25 / 2 = -0.125

M-Series Operator’s Manual 12/20/13 4-4

Page 36

Example 2: X-Axis origin offset into part 1 inch.

If you wanted the origin offset 1 inch into the part:

1. Move the Edge Finder to the left edge of the part

2. Press F1 – Next Axis until the axis field displays 'X'

3. Move the cursor to the Part Position field

4. Type -1 and press ENTER

5. Type .25 and press ENTER

6. Press SPACE until Left (-) is displayed

7. Press F10 - Set to accept the value

Axis Part Edge Finder Approach Position Diameter from X -1 0.25 Left (-)

The Position value is relative to the current position of the Edge Finder. Part position equals -1.0 since the Edge Finder is positioned 1 inch to the left (minus direction) of where you want the X-axis origin.

Another way to view the Part Position value is to assume the origin is already set at 1 inch into the part. In this case, the Edge Finder would have to move -1 inches from where the origin is to get to the left edge of the part.

The Edge Finder is approaching the part from the -X direction and has a diameter of .25 inches. Once this data is entered and F10 - Set is pressed, the X-axis DRO display will read -1.125. This means the center of the Edge Finder is sitting to the left (minus) of the origin by 1.125 inches. The X-axis origin is now 1 inch into the part.

This value is computed by: Position (Approach from) Edge Finder Diameter / 2.

Where (Approach from) is the sign of the approach direction. In other words, if the approach direction is minus, then the value is:

Position - Edge Finder Diameter / 2 = -1.0 - .25 / 2 = -1.125

M-Series Operator’s Manual 12/20/13 4-5

Page 37

Work Coordinate Systems (WCS) Configuration

Press F9 – WCS Table from the Part Setup screen to display the Work Coordinates System (WCS) menu. The Work Coordinate Systems screen provides access to reference return points, coordinate system origins, and work envelope. Make sure your Home position has been set properly. Otherwise, the positions of each coordinate system will not be in the appropriate position.

When you enter the Work Coordinate System Configuration screen, the DRO display will automatically switch over to machine coordinates as an aid to entering numbers. All the values on this screen are represented in machine coordinates.

F1 - Reference Return Points Press this key access the menu that sets the reference return points for the machine.

The reference return points are used with the G28 and G30 codes (see Chapter 12). They are specified in machine coordinates. The Z coordinate of the first reference point is also used as a Z home position by the M2, M6, and M25 codes (see Chapter 13).

F2 – Origin Use this key to access the menu for specifying the locations (in machine coordinates) of the origins

for all 18 work coordinate systems. Pressing F1 – Next Table will allow you to view the other WCS (6 per page). This menu is a convenience and is not an absolute necessity for setting work coordinate system origins nor the CSR angles.

All coordinate systems are relative to Home position that is set during control power up. Note that while in this screen, the DRO shows the actual machine position relative to Home, not the location relative to the WCS origin.

If the software option Coordinate System Rotation is unlocked, the CSR angle for each of the coordinate systems can also be set. (This is an optional feature.)

For machines configured as an Articulated Head system with the TWCS feature enabled (set via Paramter 166), the TWCS=Yes/No differentiates which WCS’s are transformed or not. See Transformed WCS later in this chapter.

M-Series Operator’s Manual 12/20/13 4-6

Page 38

F3 – Work Envelope Use the F3 – Work Envel key to specify the ‘+’ and ‘-‘work envelope locations (in

machine coordinates) used in conjunction with the G22 G code. The X, Y, Z and I, J, K parameters specified in the G22 G code are stored here, so subsequent G22 codes do not need to specify the limits unless they change.

Note: The work envelope will only work in programmed moves. You will still be able to jog outside the work envelope.

Coordinate System Rotation (CSR)

Coordinate System Rotation saves you time when setting up your part. Rather than clamping your part and indicating the edge of the material to square it with the machine axes, you can use CSR to automatically rotate the coordinate system to the angle of the part or fixture that was probed. This allows you to compensate for different orientations.

Simply clamp your part, and then probe two points along either the X or Y-axis of the material using the process described below.

M-Series Operator’s Manual 12/20/13 4-7

Page 39

F1 - Orient is used to select the orientation for the CSR measurement. There are four possible orientations, which

are: from the front (pictured above), the back, and the left and right sides.

F2 - Manual is used to determine the CSR angle without probing. The user jogs an edge finder to two positions

along one wall. These positions will be used for computing the CSR angle.

F3 - Zero Cur is used to set the CSR angle for the current WCS to zero. F4 - Zero All is used to set all CSR angles to zero. F5 – Probe Will open the probing operations menu. See Chapter 9 for details. F6 - Prev WCS and F7 - Next WCS are used to cycle through the available WCS systems. F8 – MDI The MDI menu allows you to a single line command such as: G1 X2 Y3 F20 F9 - WCS Table is a shortcut to the Work Coordinate System Configuration Screen described above.

The instructions on how to perform a CSR measurement are numbered on the screen.

Distance: The distance the X-axis (in front or back orientation) or Y-axis (in right or left side orientation) will move to probe the second point. If the distance is negative, the axis will be moved in the negative direction. Clearance Amount: The distance the Z-axis will be moved upward when moving between the first probe point and the second probe point. The clearance move will only be made when using the “Auto” option of the Movement between Points. Movement between Points can be toggled between Jog and Auto modes. In Auto mode, the clearing moves are made automatically as well as the move to the second point. In Jog mode, a prompt will be displayed in the center of the screen after the first point is probed.

Transformed WCS (TWCS=Yes)

This section only applies to Articulated Head machines with the TWCS feature enabled via Parameter 166 (see Chapter 14 for more information on setting Parameter 166). On such a machine, when a WCS has a setting of TWCS=Yes, this is then called a transformed WCS (abbreviated as TWCS).

When a TWCS is selected, the DRO will show axis positions based on the TWCS’s frame of reference. In other words, the shown positions are transformed based on the position of the B axis (5th axis). Furthermore, the WCS label will be shown as “TWCS” to indicate that the currently selected WCS is indeed transformed.

Also, when the Probing Cycles are run with a TWCS selected, the results shown will be based on the TWCS frame of reference.

Ordinary 3 axis moves types performed while running a CNC program with a TWCS selected will be automatically transformed. Such move types include:

• G0, G1, G2, G3

• Protected move probing functions M115, M116, M125, M126

• Canned Cycles G73, G74, G76, G81, G82, G83, G84, G85, G89

• M25

• Moves that involve CSR and Cutter Compensation

However, moves that will not be transformed are:

• Homing moves M91/M92

• Move to switch M105/M106

• Move axis by counts M128

M-Series Operator’s Manual 12/20/13 4-8

Page 40

Chapter 5

Tool Setup

(from Main Screen: F1 Setup ► F2 Tool)

Tool Setup allows you to specify information about the tools you will be using. Press F1 - Offset Library, to edit the Height Offset and Diameter (H and D) values, or Press F2 - Tool Library to edit the tool descriptions., or Press F3 - Tool Life to edit the Tool Life Management settings.

Offset Library (from Main Screen: F1 Setup ► F2 Tool ► F1 Offset Lib)

The Offset Library file contains the values for the Height Offset and Diameter Numbers. For example, if entry H01 has a value of -.25, a height offset of -.25 is applied when height offset 01 is referenced. If entry D01 shows a value of 1.5, the diameter offset 01 has a diameter of 1.5 associated with it.

Press F1 – Z Ref to set the Z reference height. Press F2 - Manual to manually measure tools. If you purchased the Automatic Tool Measurement (TT1) option, press F3 - Auto to automatically measure tool lengths. Press F5 - +.001 or F6 - -.001 to adjust the selected offset. If you have an automatic tool changer installed, press F7 - ATC to change tools. Press F10 - Save to save changes and exit, or ESC to exit without saving changes. If you have both purchased the Automatic Tool Measurement (TT1) option and also have an automatic tool changer installed, then you can press F4 - Auto to perform batch tool measuring, by entering a list of multiple tool numbers.

You can inspect and change any of the 200 Height Offset (H) values, and any of the 200 Diameter (D) values. In most cases you will use the automatic tool length measurement features described below to set H values, and you will enter D values manually, based on the known or measured diameters of your tools. Note that H01 and D01, H02 and D02, H03 and D03, etc. are displayed together on the same line for convenience only. The Height and Diameter Offset Numbers can be used independently; associations are made only in the Tool Library.

M-Series Operator’s Manual 12/20/13

5-1

Page 41

Height Offset

This is the distance the control adjusts Z-axis positions when tool length compensation (G43 or G44) is used with a particular H value. For example, if H001 is -1.0 and the job contains G43 H1, then the CNC software will shift all Z-axis positions down 1.0 to compensate for the shorter tool.

To edit the Height Offset entries move to the desired height offset number with the arrow keys, Page Up, Page Down, HOME, and END. You can choose to manually edit or automatically measure the value.

Height Offsets values are measured using the Z Reference position. The Z Reference position is the Z-axis position when the tip of the reference tool is touching the work surface. The reference tool should always be the longest tool.

The Height Offset value for end mills and drills is the difference between the Z-axis position when the tip of the tool is touching the work surface and the Z Reference position. The Height offset value for ball nose and bull nose cutters is the difference between the Z-axis position when the center of the tool is at the work surface and the Z reference position. Because it is not possible to position the tool in this way, you must instead move the tip of the tool to the work surface, and then manually edit the value to subtract the tool nose radius.

To manually edit a Height Offset value, simply type the desired value and press ENTER.

To manually measure Height Offset values, use the following procedure:

Establishing the Z reference position

Press F1 – Z Ref to select the Z Reference setting function. Insert the longest tool into the tool holder (you can use the jog keys or the TOOL CHECK key to assist you). Jog the tip of the tool down to the top of the work surface. Press F10 - Save to save this Z Position as the Reference Position.

Measuring each tool height (Z position for tool minus Z position for Reference tool)

Insert the desired tool into the tool holder (Jog keys or the TOOL CHECK key can be used to assist you). Jog the tip of the tool down to the top of the work surface. If the tool is a drill or end mill, press F2 –Manual Measure to measure the height. If the tool is a ball nose or bull nose cutter, press F2 – Manual Measure to measure the height, and then subtract the tool nose radius. After a tool height is measured, the next Height Offset entry is automatically selected. When the edit is complete, press F10 - Save to save the Offset Library and Exit.

Examples (assuming Z Reference = -1.5):

If the tool position is -1.75, then the tool height = -0.25 If the tool position is -1.75 and nose radius is .25, then the tool height = -0.50 If the tool position is -2.25, then the tool height = -0.75 If the tool position is -2.75 and nose radius is .125, then the tool height = -1.375

Diameter

This field tells the control the distance to adjust when cutter diameter compensation (G41 or G42) is used with a particular D value. For example, if D001 is 0.5 and the job contains G41 D1, the CNC software will adjust all X-Y positions 0.25 (half the tool diameter) to the left of the programmed tool path.

To edit the Diameter entries move to the desired diameter offset number with the arrow keys, Page Up, Page Down, HOME, and END. You must manually edit the Diameter Offset value. Type the desired value and then press the ENTER key.

You can make small adjustments to Height Offsets and Diameters using F5 - +.001 and F6 - -.001. Use the arrow keys to highlight the value to be adjusted. Press F5 - +.001 to increase the offset value by 0.001" (or 0.02 mm in Metric mode). Press F6 - -.001 to decrease the offset by the same amount. If the cut parts are undersized, use F5 - +.001 to cut less material. If the cut parts are oversized, use F6 - -.001 to cut more material.

M-Series Operator’s Manual 12/20/13

5-2

Page 42

Automatic Tool Measurement

Z-minus single-surface probing, using the TT-1 tool touch-off post, is available in the Tool Offset Library.

First Time Setup

Make sure the proper parameters are set as per Chapter 9 and Chapter 14, and the detector is plugged in and is at the correct location on the table! When first testing the TT-1, hold the TT-1 in hand and manually touch the unit to the tool to confirm correct electrical connection and parameter setup.

WARNING

Setting the Z Reference: Using the longest tool for the job to be run or the designated reference tool, press F1- Z Ref, then F3 and then CYCLE START. The Z-axis will then move down until the tool touch-off is detected. The Z reference will be set

at that position. Parameter 3 bit 1 is used to set Z reference to Z home position. See the parameter section in Chapter 14 for more info.

Setting the Tool Height Offsets:

Pressing F3 – Auto Measure and then CYCLE START at the prompt will cause the Z-axis to move down until the tool touch-off is detected; the resulting tool length will be entered in the table (same as with F2 - Manual). The Z-axis then returns to its home position.

If Parameter 17 has been set to the number of a valid return point (1 or 2), the F3 – Auto Measure option will move the X and Y axes to that return point before moving Z down. Return point 1 is the G28 position from the Work Coordinate System Configuration screen (see Chapter 4). Return point 2 is the G30 position on that screen. If Parameter 17 is zero (0), the X and Y-axes will not move before Z moves down. In this case you must be careful to jog the machine directly over the detector before pressing F3 – Auto Measure.

Incorrect setup may cause damage to the machine, tool and/or cause injury to the operator.

Note: SHIFT+F3 can be used to override any return point movement in cases where parameter 17 is set to use it. This is helpful for measuring tools wherein the height measurement is not taken from the center point of the tool.

Batch Tool Height Offset Measurement Process:

If you have both purchased the Automatic Tool Measurement (TT1) option and also have an automatic tool changer installed, then you can press F4 - Batch to measure multiple tools in one process. After pressing F4 - Batch, you will be prompted with the following dialogue box:

After entering a list of tool numbers, you can press CYCLE START to perform the batch tool measurement process. This process is similar to the single tool height offset measurement (accessed via F3 – Auto Measure) but will do multiple tools in one shot.

M-Series Operator’s Manual 12/20/13

5-3

Page 43

Setting up Tool Height Offsets

NOTICE

Using a Probe as the Reference Tool

Before you set the Z Reference, make sure the probe Tool # is entered into Parameter 12 on the Machine Parameters screen. Make sure that Parameter 17 on the Machine Parameters screen contains a 0. Follow these steps to probe Z Reference:

1. Load the probe into the machine.

2. Jog the probe over the desired reference surface and press F1 – Z Ref.

3. Press F3 and then CYCLE START; the probe will find the Z Reference.

At this point, the Z Reference is now entered into the Offset Library and is the reference height for all other tools. Remove the probe and measure any other tool offsets manually as described earlier in this chapter.

Measuring Each Tool Offset Using a Fixed Detector

Before measuring any tool height, make sure you enter the probe or reference tool-measuring location. Do this by entering a reference point number (1 or 2) into Parameter 17 and entering the detector position as the corresponding Reference Return Point on the WCS Configuration screen. Otherwise, the machine may traverse to a location that could damage the probe or reference tool. Also remember that if Parameter 17 is zero (0), the X and Y-axes will not move before Z moves down. Also be sure that parameter 44 is set correctly. This is the input number for the TT1. Now that a permanent location has been set, do the following:

Load reference tool (preferably the longest tool) and highlight its corresponding Height Offset # using the up or down arrow keys. Press F1 – Z Ref, then F3 – Auto Measure and then CYCLE START to set the Z reference using this tool. The X and Y-axes will traverse to the preset location, and then Z will move down until the tool is detected and the Z reference will be set. Load the next tool. Highlight the desired Height Offset # on screen using the up or down arrow keys. Press F3 – Auto Measure and then CYCLE START. The X and Y-axes will traverse to the preset location, and then Z will move down until the tool is detected. Once the detector is triggered, the tool offset will show on the screen. A negative offset means the tool is shorter than the reference tool.

Once all of the tool offsets have been measured, press F10 - Save to save them. Otherwise, press ESC to cancel any changes.

Before manually jogging any probe to a position, make sure the machine Feedrate is turned down (less than 10 in/min) or damage to the probe may result!!!

M-Series Operator’s Manual 12/20/13

5-4

Page 44

Tool Library

Pres

PresPres

Pres

s CYCLE START to start job

s CYCLE START to start jobs CYCLE START to start job

s CYCLE START to start job

Clear

Clear Clear

Clear

FFFF

1111

Clear

Clear Clear

Clear

FFFF

2222

Tool

Tool Tool

Tool

Bin

BinBin

Bin

Ht.

Ht.Ht.

Ht.

Dia.

Dia.Dia.

Dia.

Coolant

CoolantCoolant

Coolant

Spindle

SpindleSpindle

Spindle

Speed

SpeedSpeed

Speed

Description

DescriptionDescription

Description

Tool Library

Tool LibraryTool Library

Tool Library

(from Main Screen: F1 Setup ► F2 Tool ► F1 Tool Lib)

WCS #1 (G54) Current Position (Inches)

WCS #1 (G54) Current Position (Inches) WCS #1 (G54) Current Position (Inches)

X +4.0000

X +4.0000X +4.0000 Y +2.0000

Y +2.0000

Y +2.0000Y +2.0000 ZZZZ

----

T001

T001 000 H001 D0001 FLOOD

T001T001

T002

T002 000 H001 D0001 FLOOD CW 500

T002 T002 T003

T003 000 H001 D0001 FLOOD CW 500

T003 T003 T004

T004 000 H001 D0001 FLOOD CW 500

T004 T004 T005

T005 000 H001

T005 T005 T007

T007 000 H001 D0001 FLOOD CW 500

T007 T007 T008

T008 000 H001 D0001 FLOOD CW 500

T008 T008 T009

T009 000 H001 D0001 FLOOD CW 500

T009 T009 T010

T010 000 H001 D0001 FLOOD CW 500

T010 T010

0.5000

0.50000.5000

000 H001 D0001 FLOOD CW 500

000 H001 D0001 FLOOD 000 H001 D0001 FLOOD 000 H001 D0001 FLOOD CW 500

000 H001 D0001 FLOOD CW 500000 H001 D0001 FLOOD CW 500 000 H001 D0001 FLOOD CW 500

000 H001 000 H001 000 H001 D0001 FLOOD CW 500

000 H001 D0001 FLOOD CW 500000 H001 D0001 FLOOD CW 500 000 H001 D0001 FLOOD CW 500

000 H001 D0001 FLOOD CW 500000 H001 D0001 FLOOD CW 500

D0001 FLOOD CW 500

D0001 FLOOD CW 500 D0001 FLOOD CW 500

CW 500

CW 500 CW 500

Job Name :

Job Name : bbbbracket.cnc

Job Name : Job Name : Tool :

Tool :

Tool : Tool : Feedrate : 100%

Feedrate : 100%

Feedrate : 100%Feedrate : 100% Spindle : 0 M

Spindle : 0 M

Spindle : 0 M Spindle : 0 M

Stopped

StoppedStopped Waiting for PLC operation

Waiting for PLC operation

Waiting for PLC operationWaiting for PLC operation

racket.cnc

racket.cncracket.cnc

T001 H001

T001 H001T001 H001

Save

Bin

BinBin

All

AllAll

Save Save

The definitions in the Tool Library associate tool (T) numbers with height offset (H) and diameter (D) numbers, the default coolant type, spindle direction, and spindle speed for the tool, and a text description of the tool. This information is used by the Intercon-programming package (described in Chapter 10) to provide defaults whenever a tool change is selected. For enhanced ATC features, the (T) numbers are also associated with bin numbers. See Chapter 14 for more information about enhanced ATC features (parameter 160).

Note: If enhanced ATC features are not on, the cursor cannot be moved into the bin column and the message “Bin fields are locked.” will appear where the tool in spindle display is located. In addition, the F1 – Clear Bin and F2 – Clear All keys only appear if enhanced ATC features are on.

You can inspect and change any of the 200 tool definitions. To edit a Tool Library definition move to the desired tool number with the arrow keys, Page Up, Page Down, HOME, and END. To change Height Offset numbers, Diameter numbers, default spindle speed values and the tool description, type a new value into the field and then press ENTER. To change the default spindle direction and coolant press SPACE to cycle through the possible values. When the changes are complete press F10 - Save to save the Tool Library and exit.

Bin

This field specifies which bin location, or ATC carousel position, that the tool is occupying. Valid values are –1 (shown as dashes “---“) through the maximum number of tools specified by machine parameter 161. A value of 0 indicates that the tool is in the spindle. The F1-F2 keys will work when the cursor is in the Bin column. F1 - Clear Bin – places dashes “---“into the bin field (same as entering –1). F2 - Clear All – places dashes into every bin field.

Note: For enhanced ATC applications, the bin numbers will be updated when tool changes are completed. For random, or arm type tool changers, tools in the spindle are placed into the bin where the next tool is picked up, and not necessarily from the bin which it was originally taken.

M-Series Operator’s Manual 12/20/13

5-5

Page 45

Height

This field specifies a default Height Offset (H) number to use with each tool. Possible values are 1 to 200. Intercon uses this information to provide a default H value at each tool change. The CNC software also uses this information to correct for the length of the tool that is used to establish the Z-axis position in Part Setup (see Chapter 5).

Diameter

This field specifies a default Diameter (D) number to use with each tool. Possible values are 1 to 200. Intercon uses this information to provide a default D value at each tool change. To change the value type a new number and press ENTER.

Coolant

This field specifies a default coolant type to use with each tool. Possible values are FLOOD, MIST, or OFF. Intercon uses this information to automatically insert M7 or M8 after a tool change. To change the value, press

SPACE until the desired value is shown.

Spindle

This field specifies a default spindle direction to use with each tool. Possible values are CW, CCW, or OFF. Intercon uses this information to automatically insert M3 or M4 after a tool change. To change the value, press

SPACE until the desired value is shown.

Speed

This field specifies a default spindle speed to use with each tool. Possible values are 0 to 500000. Intercon uses this information to automatically insert an S code after a tool change. To change the value, type a new number and press ENTER.

Description

This field contains a text description of the tool. The description will appear in a prompt message on the screen when the CNC software reaches a tool change (M6).

M-Series Operator’s Manual 12/20/13

5-6

Page 46

Tool Life Management menu (from Main Screen: F1 Setup ► F2 Tool ► F1 Tool Life)

The Tool Life Management feature allows you to set up each tool’s pre-determined life, and have its usage tracked and monitored for end-of-life condition. By default, Tool Life Management is turned off, but can be enabled for each tool individually.

F1 – Show/Hide Unmanaged. This key toggles between including and excluding those tools that are unmanaged by Tool Life Management. A tool is unmanaged if its Total Life field is set to value 0 (Off ). F2 – Sort Recent. This key sorts the list according to the tools whose Total Life and/or Used field were most recently modified by tool usage in a job run or by edits done in this menu.

F3 – Sort Tool #. This key sorts the list ordered by Tool Number. F4 – Sort Remaining. This key sorts the list ordered by the Life Remaining. F10 – Save. Saves changes.

A tool can be set up for automatic management by setting its Mode to Auto and setting its Total Life to a non-zero value. The following table shows the effects of monitored tool activity on tools that are set up for automatic management.

Automatic Management: Mode = Auto and Total Life is more than 0 Type Units Tool Activity that is monitored Effect on the ‘Used’ field

Drill Cycles downward Z plunge at feedrate at

a unique XY location

Drill Inch/mm downward Z plunge at feedrate at

a unique XY location EM (End Mill) EM (End Mill)

Cycles Tool Change ‘Used’ field will be incremented by 1

Inch/mm sideways XY feedrate moves (non-

rapid)

‘Used’ field will be incremented by 1 Cycle Total downward Z distances minus the overlaps will be added to the ‘Used’ field

Cycle XY distance will be accumulated in the ‘Used’ field

M-Series Operator’s Manual 12/20/13

5-7

Page 47

Detailed description of each field is as follows.

Type

This is the type of tool – either Drill or EM (end mill). Whent the Mode field is set to Auto, this field determines the type of tool activity that will be automatically tracked and monitored for the purpose of accounting for consumed tool life. (See the Automatic Management table above.) Note that if the tool is a Bore or a Tap, you should select Drill.

Total Life

This field specfies the total amount of tool life. A value greater than 0 enables Tool Life management for the tool. A value of 0 (Off) excludes the tool from Tool Life management. Such a tool is called an “Unmanaged” tool. Unmanaged tools can be shown or hidden by pressing F1. The units of this field is specified in the Units field.

Used

This field is the amount of consumed tool life. When a new tool is first set up, you should initialize this field to 0 indicating zero usage. If the Mode field is set to Auto, this field will automatically be modified during a job run to reflect the accumulated tool usage. The units of this field is specified in the Units field.

Remaining (non-edit)

This is the display of the remaining amount of tool life.

Units

This specifies the units (either distance or Cycles) that will be used and displayed for the Total Life, Used, and Remaining fields. Distance is specified with mm or Inches (as set in the Control Configuration menu – see Chapter

14).

Mode

This specifies the update mode of the Used field -- either Auto or Manual. If this field is set to Auto, then tool activity is montiored during a job run for tool usage which will be automatically accumulated in the updated Used field. (See the Automatic Management table above.)

If this field is set to Manual, no such automatic updates will take place on the Used field. Rather, updates to the Used field will be dependent upon user variable modifications programmed in the G-code program being run. (See the section Tool Life Management – Using G-Code User Variables later in this chapter.)

Description

This field contains a text description of the tool. The description will appear in a prompt message on the screen when the CNC software reaches a tool change (M6) during a job run.

M-Series Operator’s Manual 12/20/13

5-8

Page 48

Tool Life Management – Effect on Job Run and Backplot

At Start of Job

Tool life expirarations will be checked at the beginning of a job run. If any managed tools are expired at the beginning of a job, the following dialog will show up and you will have one of 3 choices to make:

When a job is first started, the CNC software will not yet know which tools are going to be used in the job until the job is successfully completed. Therefore, the tools listed here will be the list of all expired tools even if they are not going to be used in the job.

At Job Restart

Tool life expirations are also checked upon job restart (i.e. upon encountering M2 or M102). If any tool(s) expired during the previous job run (previous to the M2 or M102), then the dialog that is displayed is similar to that shown above except that the expired tools listed will only be the ones that were used in the job.

At End of Job

When tool life expires during a job, such an event will not cancel the job. Instead, upon successful end of the job the following dialog will be displayed and you will have an opportunity to quickly get to the Tool Life Management menu:

This end-of-job dialogue will show only the expired tools that were used in the job.

Using Backplot Graphics to Predict Tool Expirations

You can use Backplot Graphics as a way to predict ahead of time whether or not one or more tools will expire during a job. Simply press F8 Graph at the Main Screen or in the Load menu. If the job being graphed will result in an expired tool if it was actually run, then the following message will show up:

M-Series Operator’s Manual 12/20/13

5-9

Page 49

Tool Life Management – Using G-Code User Variables

If a tool’s Mode field is set to Manual, there will be no updates to the Used field of the Tool Life data during a job run, unless the job’s G-code is programmed to modify it.

The following is an example of how a G-code program would modify tool life data. Assuming tool T23’s Mode is set to Manual, and its Units is set to Cycles, the following G-code will increment T23’s Used Life field by 1 after completing the example_cycle.cnc.

M6 T23 ; change tool to T23 M98 "example_cycle.cnc" L1 ; run the cycle 1 time IF #4201 || #4202 THEN GOTO 100 ; skip to N100 if in backplot or search mode IF #4120 < 1 || #4120 > 200 THEN GOTO 100 ; skip to N100 if T number is not valid #[19000+[#4120-1]*5+2] = #[19000+[#4120-1]*5+2] + 1 ; increment current tool's Used Life by 1 cycle N100 ; destination of goto’s

See Chapter 11 for more information about the use of User or System Variables.

M-Series Operator’s Manual 12/20/13

5-10

Page 50

Chapter 6

Running a Job

To start the currently loaded job, go to the Main Screen and press the CYCLE START button on the jog panel. If your control is not equipped with a jog panel, press ALT-S on the keyboard.

Active Job Run Screen with G-code Display

If the Run-Time Graphics option is set to Off, the following screen is displayed while a job is running:

On this screen, the following F-keys are available:

F1 – Feed (-1%) F2 – Feed (+1%) F3 – Repeat On/Off

F4 – Skips On/Off

F5 – Auto

F6 – Stops off

F7 – Feed Hold F8 – Graph

F9 – Rapid On/Off

For information on other keys that are available while a job is running, see Chapter 2.

M-Series Operator’s Manual 12/20/13

Decrease feedrate override by 1%. (Available only if keyboard jogging is active.) Increase feedrate override by 1%. (Available only if keyboard jogging is active.) Toggle the repeat feature for part counting. For more information, see F3 under the Run Menu section later in this chapter. Enable/Disable block skips. For more information, see F4 under the Run Menu section later in this chapter. This key will only appear in Single Block mode. When you press this key, it turns on Auto mode and disables Single Block mode. Once Auto mode is turned on, Single Block cannot be re-enabled unless you stop the job. For more information, see F5 under the Run Menu section later in this chapter. This key will only appear if Optional Stops is on. When you press this key, it turns off Optional Stops. Once Optional Stops is turned off, it cannot be re-enabled unless you stop the job. For more information, see F6 under the Run Menu section later in this chapter. Turn feed hold on/off. (Available only if keyboard jogging is active.) Switch to run-time graphics screen. This key only appears if the job was started with the run-time graphics option turned on. Turn rapid override on/off.

6-1

Page 51

Run-Time Graphics Screen

When a job is running with Run-Time Graphics set to On, the following screen is displayed:

The following keys are available while the job is running in Run Time Graphics.

F7 – Clear F8 – G-Code F9 – Trail On/Off

Clears the trail up to the tool’s current position in the program. Switch to the Job Run Screen with G-Code display. Turn on/off the tool trail display.

Canceling a Job in Progress

There are three conventional ways to cancel a currently running job (CNC program). When a job is canceled using any of the following methods, the job's progress will be recorded. This allows the user to restart the job using the Resume Job option or the Search and Run option.

CYCLE CANCEL pressing this key while a job is running will cause the control to abort the job

currently being run. The control will stop movement immediately, clear all M-functions, and return to the main screen. Hitting the escape key on the keyboard is equivalent to hitting “CYCLE CANCEL.”

TOOL CHECK Pressing this key while a job is running will cause the control to stop the normal

program movement. In addition, the Z-axis will be pulled to its home position and all Mfunctions will be cleared. The control will automatically go to the resume job screen.

EMERGENCY STOP (E-Stop) Pressing the EMERGENCY STOP button, while a job is running,

will cause the control to abort the job currently being run. The control will stop movement immediately, clear all M-functions, and return to the main screen. Also, the power to all axes will be released.

M-Series Operator’s Manual 12/20/13

6-2

Page 52

Resuming a Canceled Job

If a job is canceled using one of the methods described above, it can be resumed in one of three ways:

CYCLE START Pressing the CYCLE START button will restart the job at the BEGINNING of the

part program.

F1 - Resume Job (Located in F4-Run menu) Restart the canceled job at or near the point of

interruption. See the next section in this chapter entitled “Run menu” for more information.

F2 - Search (Located in F4-Run menu) Restart at a specified point in the part program. See the next

section in this chapter entitled “Run menu” for more information.

Run menu

Press F4 - Run from the main screen to access the Run menu. From this menu, the operator can restart a canceled job or change the way the job will run.

F1 - Resume Job Access the resume job screen by pressing F4 - Run on the main screen to go to the

run screen, and then pressing F1 – Resume Job in the run screen to go to the resume job screen. If the job was canceled by pressing TOOL CHECK, the control will go to the resume job screen automatically. From this screen, the user can modify tool offsets and the tool library, turn block mode on and off, turn optional stops on or off, graph the partially completed job, or start the partially completed job.

The resume job option is not always available. The following situations will cause the resume job option to be unavailable:

• Loading a new job.

• Running a job to completion.

• Parse errors in the job.

• Editing or reposting the job file.

• Loss of power while a job is running.

M-Series Operator’s Manual 12/20/13

6-3

Page 53

F2 – Search Invoking this option will bring you to the “Search and Run” menu. This menu will allow

you to specify the program line, block number, or tool number at which execution of a program is to begin. Program lines are numbered from the top of the file down with the first line numbered

1. To enter a block number, place an "N" in front of the number. To enter a tool number, place a "T" in front of the number. Pressing CYCLE START from here would start the program at the point you specified.

An extra option unique to the “Search and Run” screen is the F1 – Tool Change “Do Last Tool Change” function. This key toggles the tool change option as shown on screen. A "YES" tells the control to perform a tool change so that the tool specified for the line or block has the tool indicated in the program. A "NO" uses the currently loaded tool, regardless of what tool is specified for the line or block being searched.

NOTE: You cannot search into a subroutine.

F3 – Repeat On/Off This key toggles the repeat feature for part counting. When part counting is in

effect and Repeat is on, the job will be automatically run again until the specified number of parts has been run. The On or Off label indicates the state to which the repeat feature will toggle to when pressed. It does not indicate the current state. The current state is indicated in the user window above.

The Part Count: prompt is used to set the Part count. Positive values set the part counter to count up and negative values configure the part count to count down. For example, if 10 is entered in the Part Count prompt, the Part Cnt in the status window changes to 10 and the Part # changes to 0 with an upward arrow indicator. When a job is run and then completes, the Part # will increment to 1. If repeat is on, the job will automatically start again and keep running until the Part # has reached the Part Cnt. If a –10 is entered in the Part Count prompt, the Part Cnt in the status window changes to 10 and the Part # changes to 10 with a downward arrow indicator. When a job is finished, the Part # will decremented to 9. If repeat is on, the job will automatically start again and keep running until the Part # has reached 0.

F4 - /Skips On/Off This function toggles the block skip feature. When block skipping is on, G-code

lines that start with a forward slash character ‘/’ are skipped, i.e., they are not processed. Note that because of the way a job is processed (in a pre-processed buffered fashion) the effect of this key may be delayed if you press it while a job is running. The On or Off label indicates the state to which the /Skips feature will toggle to when pressed. It does not indicate the current state. The current state is indicated in the user window above.

F5 - Block Mode Turns single block mode on and off. This is similar to pressing AUTO/BLOCK. If

Single Block mode is on, the CNC software will stop after each block in your part program and wait for you to press CYCLE START. Note that Auto mode is the default mode. If you use this key to turn on Single Block mode and then run a job, Auto mode will be re-instated when the job ends. The current state of this setting is indicated in the user window above.

F6 - Optional Stops Turns optional stops on and off. If optional stops are on, any M1 codes that

appear in your program will cause a wait for CYCLE START (just like M0). If optional stops are off, M1 codes will be ignored. Note that the default mode for Optional Stops is off. If you use this key to turn on Single Block mode and then run a job, Optional Stops will be set to off when the job ends. The current state of this setting is indicated in the user window above.

M-Series Operator’s Manual 12/20/13

6-4

Page 54

F8 – Graph Graphs the part. For more information, see the "F8 - Graph" section in chapter 3. If this

feature is invoked from the Run and Search screen or the Resume Job screen, then the graphics will show exactly where the searched line or block begins. Dotted lines indicate the portion of the part that is skipped. Solid lines indicate the portion of the part that will be machined.

F9 – Rapid On/Off This function key toggles Rapid Override. The On or Off label indicates the state

to which the Rapid Override feature will toggle when pressed. In the Rapid Override On state, the speed of rapid moves (G0) can be adjusted by the Feedrate Override knob. In the Rapid Override Off state, the speed of rapid moves will be at full speed (max rate).

F10 – RTG On/Off This function key toggles the Run-Time Graphics option. If the option is turned

on, Run-Time Graphics automatically starts when the CYCLE START button is pressed. This option must be turned on for Run-Time Graphics to be used. If the option is turned off, RunTime Graphics cannot be started while a job is running.

Power Feed

Press F4 - Feed from the Setup menu to access the Power Feed screen. This screen is used to command axis movement. All the operations available on the Power Feed screen may also be performed in MDI with the appropriate M and G codes.

F1 - Absolute Power Feed Press F1 - ABS to move an axis to an absolute position, at a specified

feedrate.

F2 - Incremental Power Feed Press F2 - INC to move an axis an incremental distance, at a specified

feedrate.

F3 - Free XY Press F3 - Free to release power to the X and Y motors, allowing you to use your

machine manually for these two axes.

F4 - Power XY Press F4 - Power to apply power to the X and Y motors, allowing you to use your

machine with the jog panel for these two axes.

M-Series Operator’s Manual 12/20/13

6-5

Page 55

M-Series Operator’s Manual 12/20/13

6-6

Page 56

Chapter 7

The Utility Menu

To get to the Utility Menu, press F7 - Utility at the CNC software Main Screen. The model will vary depending on your M-Series Control model.

F2 – Restore Report This option is used primarily for restoring a system configuration from a previously

saved report.zip file (See F7 – Create Report).

F3 – Backup Files This creates an archive file “cnc_backup.zip” containing CNC program files, Intercon

part program files, MillWrite engraving files, and digitized output files from the following directories and their subdirectories: ncfiles directory, c:\intercon, c:\mw, and any other directories mentioned in the pathm.ini configuration file.

F4 – Restore Files Use this option to restore the data previously backed up with F3 – Backup Files. (Note

that this feature will not work with backups created by control software prior to version 3.04.)

M-Series Operator’s Manual 12/20/13

7-1

Page 57

F5 – File Ops Use this menu to perform file and directory operations such as: Importing and Exporting

(copying) files to and from the control, rename or delete files, create or delete directories.

F1 – Toggle

F2 – All /None

F3 – Import/ Export F4 – Edit

F5 – Refresh

F7 - Rename

F8 - New Dir

F9 - Delete

Page Up

Page Down

End Home

Arrow Keys

Press once to select or press again to unselect a single file.

Press once to select all or press again to unselect all files.

Import or Export selected files.

Opens selected file in editor.

Refresh file list. Use after inserting a new USB storage device

Rename selected file or directory.

Create a new directory in the current folder.

Deletes selected file or directory.

Move the cursor backward one page.

Move the cursor forward one page.

Select the last file in the list.

Select the first file in the list.

Move the cursor in the selected direction.

M-Series Operator’s Manual 12/20/13

7-2

Page 58

F6 – User Maint

Use this menu to perform user maintenance such as checking an axis for excessive drag or setting backlash

F1 – Drag The Drag Factor utility is used to determine if an axis has an excessive amount of drag. To

run a drag test, use the F1 key to select the axis which you wish to test, position the axis at or near the home position and press CYCLE START. The axis will move back to the home switch then traverse the entire range of travel for the axis moving to the opposite limit and returning to home while moving the slow jog rate. If excessive friction (drag) is encountered an error message will be displayed. When the test completes, use F8-Graph to display the results. The red horizontal lines indicate the bounds acceptable limits for the machine as it is currently configured.

F2 - Lash (Backlash Compensation) In order to insure an accurate measurement always set the backlash

compensation in the control to zero before attempting to measure the physical lash in an axis.

F7 – Create Report Generates a backup of system configuration files called report.zip and copies it to the

specified location. Your dealer may then use this file for servicing and troubleshooting purposes. To restore the configuration files from the report disk, press F2 – Restore Report from the Utility menu.

F8 – Options Shows the software options that you have purchased or added to your control. On this screen

you can also enter unlock codes for software options that you have purchased. This page will also display the PLC programs, PIC type, and System ID #.

F9 – Logs Shows the messages and errors that have been logged by the control.

F1 – Errors Displays the error/message log. Use PgUp, PgDn, Home, & End to view and ESC to exit.

F2 – Stats Displays counts of errors logged. Use PgUp, PgDn, Home, & End to view and ESC to exit. F3 – Export Exports the log to a destination of your choosing.

M-Series Operator’s Manual 12/20/13

7-3

Page 59

M-Series Operator’s Manual 12/20/13

7-4

Page 60

Chapter 8

Digitize

(F9 from Main Menu)

The Digitize feature of the CNC software can be used to digitize surfaces in a variety of scenarios. The digitizing process creates a file with M & G codes that represent the digitized surface. If the digitizing probe tip is chosen to match the milling cutter size, the digitized file can be loaded and run to produce an exact copy of the digitized part.

F1 – Grid F2 – Radial F3 – Contour F4 - Probe F6 – Dig to CAD F8 – Wall Following

M-Series Operator’s Manual 12/20/13

Digitize rectangular surface area. Digitize inside of a bore. Digitize inside or outside contour. Select from the Probing Cycles (See Chapter 9 of this manual). Export digitized files for use with a CAD/CAM system. Digitize inside and/or outside contour .

8-1

Page 61

Grid Digitize

(F1 from Digitize Menu)

Grid Digitize Run Setup

To set up a digitizing run, edit the parameters shown and then press CYCLE START. The control will move through the area to be digitized in a rectangular pattern. At each X-Y point in the pattern, it will measure the Z height of the sample surface, and record the coordinates in the data file.

Digitizing begins at the current tool position when the CYCLE START button is pressed. This position should be in one corner of the digitize area, at a Z position higher than any point on the surface.

Grid Digitize Parameters

Type: This sets the algorithm for digitizing: either regular Grid or Surface Following.

X Patch Length: The length of the area to be digitized, along the X-axis. A positive value will cause digitizing to proceed in the X+ direction from the starting point; a negative value will cause digitizing to proceed in the Xdirection. If the value is 0, then digitizing will collect just one stripe along Y.

X Step Over: The distance to move between points on the X-axis. A smaller value should be used for a fine digitize along the X-axis. A larger value should be used for a rough digitize along the X-axis. This distance should be a positive incremental value.

Y Patch Width: The width of the area to be digitized, along the Y-axis. A positive value will cause digitizing to proceed in the Y+ direction from the starting point; a negative value will cause digitizing to proceed in the Ydirection. If the value is 0, then digitizing will collect just one stripe along X.

M-Series Operator’s Manual 12/20/13

8-2

Page 62

Y Step Over: The distance to move between points on the Y-axis. A smaller value should be used for a fine digitize along the Y-axis. A larger value should be used for a rough digitize along the Y-axis. This distance should be a positive incremental value.

Z Maximum Depth: The maximum distance the Z-axis moves below the starting height. If the probe does not contact the surface at the maximum depth, that data point will be recorded as being at the maximum depth, and digitizing will proceed with the next point.

Z Step Up: The distance the Z-axis moves up after making contact, before the control attempts to move X or Y. A small value should be used when digitizing parts with gentle slopes; a larger value should be used when digitizing parts with many steep walls.

Axis to Move First: The axis (either X or Y) which moves all the way across the digitize area with each pass.

Digitize File Name: The base name of the output file in which the digitize data is stored. An extension of .dig will automatically be appended to the name for replay as a CNC job.

Replay Feedrate: The feedrate to include with the G1 command on the first line of the data file. If the data file is run as a CNC program, this is the feedrate at which the machine will retrace the digitized surface.

Multiple Patch: Indicates whether or not this digitizing is a continuation of an earlier digitizing. Choose NO if the current digitizing is the first or only digitize run for the part to be digitized. Choose YES if the current digitizing is not the first digitize run for the part. If Yes is selected, specify the name of a digitize file of a previous multiple patch.

Replay Pattern: Indicates the replay movement pattern. If ZIG ZAG is selected, the replay pattern will alternate between positive and negative directions on each successive pass. If ONE WAY is selected, the replay pattern will maintain a constant "one-way" direction throughout the playback.

Probe Diameter: Indicates the probe tip diameter.

M-Series Operator’s Manual 12/20/13

8-3

Page 63

Grid Digitize Notes

1. A guide to the possible grid digitizing paths is as follows:

2. A digitizing patch can be located anywhere in the coordinate system. The digitizing starting point is referenced from the part zero. For example, setting up digitizing, as shown in the figure on the right below, will record the first point at (X5, Y5, Z1) and the last point at (X7, Y7, Z1). If the digitizing replay starting point is desired to be at the part zero be sure to set the part zero equal to the digitizing start point, as shown in the figure on the left below. This orientation will record the first point at (X0, Y0, Z0) and the last point at (X2, Y2, Z1). For more information on part setup see Chapter 4.

M-Series Operator’s Manual 12/20/13

8-4

Page 64

3. A good technique for calculating Z maximum depth is to touch off the lowest surface of the part to be digitized and set the part zero's Z value to Z0. Then jog the probe tip to a point higher than the highest surface of the part to be digitized. Note the displacement in the Z-axis. Again, set this Z height to Z0 and use the noted displacement for the Z maximum depth.

4. Multiple patches are useful in the following situations: completing a canceled digitize run, digitizing parts with large areas that contain nothing to be digitized (shown below), and patching vertical walls to eliminate scallops caused by the cutting tool.

The drill shown in the previous example is L-shaped. Therefore, it can be digitized faster and more efficiently using three rectangular patches than digitizing the complete area with a single patch.

Digitizing the entire part and then adding multiple small patches along the walls can avoid vertical wall scalloping. If a vertical wall extending along the X axis needs to be cleared of scallops, just add a small patch running the length of the wall. Set the “Axis to Move First” parameter to Y. This will clear the scallops.

M-Series Operator’s Manual 12/20/13

8-5

Page 65

Radial Digitize

(F2 from Digitize Menu)

Setting up a Radial Digitize Run

To set up a digitize run, edit the parameters shown. Jog the probe tip to the starting height and to the center of the bore to be digitized. Then press F1 - Center to define the center position for digitizing. This center position will be used as the center of all radial digitizing runs until you leave the radial digitize menu or redefine the center. If you are using a full angle, you can now press CYCLE START to begin digitizing. If you have specified partial angle, press F2 - Partial to define the partial angle (see setting the partial angle section in this chapter). After defining the partial angle, pressing CYCLE START will start the digitize run.

WARNING: The probe must be able to retreat to the center from any position on the digitize surface. If the digitize surface contains features that do not allow for the probe to exit after entering, a probe crash may occur! See radial digitize note 2 later in this section.

Radial Digitize Parameters

Containment Radius: The maximum distance from the center position to look for a digitize data point. This parameter is used to contain the probe within a circle with this radius centered at the center position. If the probe does not contact the surface before reaching the maximum radius that data point will be recorded as being at the maximum radius, and digitizing will proceed with the next point.

M-Series Operator’s Manual 12/20/13

8-6

Page 66

Z Patch Depth: The depth of the patch to be digitized, along the Z-axis. A positive value will cause digitizing to proceed in the Z+ direction from the starting point; a negative value will cause digitizing to proceed in the Zdirection.

Z Step: The distance to move between points on the Z-axis. A smaller value should be used for a fine digitize along the Z-axis. A larger value should be used for a rough digitize along the Z-axis. This distance should be a positive incremental value.

Outer Stepover: The distance to move between points on one contour. A smaller value should be used for a fine digitize along any one contour. A larger value should be used for a rough digitize along any one contour. This distance should be a positive incremental value.

Replay Pattern: Indicates the replay movement pattern. If Zigzag is selected, the replay pattern will alternate between positive and negative angle directions (CW and CCW) on each successive contour. If CW or CCW is selected, the replay pattern will maintain a constant angle direction throughout the playback.

Digitize File Name: The base name of the file in which the digitize data is stored. The file has an extension of .dig for CNC replay.

Containment Angle: Indicates whether or not the digitizing is to follow a full circle or a partial sector. Choose Full if 0 to 360 degrees is desired. Choose Partial if some other angles are needed. These partial angles can then be changed later (see setting the Partial Digitizing Sector Setup section that follows).

Multiple Patch: Indicates whether or not this digitizing is a continuation of an earlier digitizing. Choose No if the current digitizing is the first or only digitize run for the part to be digitized. Choose Yes if the current digitizing is not the first digitize run for the part. If Yes is selected, specify the name of a digitize file of a previous multiple patch.

Move Between Levels: This field is enabled only if Partial and CCW or CW option is selected. It indicates the move between Z levels on replay of a partial sector radial digitize file. This move may now be done in three different ways: Clearance, which goes to the clearance height as in previous versions, Center, which goes to the digitizing center and then to the Z level of the next pass, and Direct, which goes directly to the starting point of the next pass.

Clearance Height: This field is enabled only if Partial, CCW or CW replay pattern, and Clearance Move type option is selected. This distance indicates the clearance height needed to move the cutter from the end of one contour to the beginning of the next contour. This distance should be a positive value.

M-Series Operator’s Manual 12/20/13

8-7

Page 67

Radial Digitize Notes

1. A guide to possible radial digitizing paths is as follows:

2. When radial digitizing, make sure the probe can fully retract to the center position without obstructions. Observe the two parts below. The cross section on the left has no obstructions that could keep the probe from full retraction to the center position. The cross section on the right does not allow the digitizing to retract to the center in Area A. This area will cause a probe crash; single patch digitizing of parts such as this should be avoided. Use 2 or more patches to digitize the part on the right (in this case, you could divide the part in half horizontally, and do each half separately).

M-Series Operator’s Manual 12/20/13

8-8

Page 68

Partial Digitizing Sector Setup

If you set the Radial Digitize Containment Angle to “Partial” then you must set up the Digitizing Setup by pressing F2 - Partial from the CNC software Radial Digitize Screen.

The partial sector can be setup one of two methods:

One method is by editing the start and end angles directly. The start angle is referenced from zero degrees and defines the beginning of the digitizing sector. The end angle is referenced from zero degrees and defines the end of the digitizing sector.

The second method involves jogging the probe tip and touching off the digitize surface. By moving the probe tip to positions on the digitizing surface, one can set the angles. To set the start angle, jog the probe tip to the position on the digitizing surface where the digitizing is to begin and press F1 - Start to define this as the start angle. * Notice that the picture of the sector and the start angle's value change to reflect these settings. To define the end angle, follow the procedure above but press F2 - End instead to set the end angle.

Regardless of the method used to define the start and end angles, pressing F10 - Save saves the angles and exits back to the radial digitize menu. Pressing ESC will return to the radial digitize menu without making changes to the start and end angles.

M-Series Operator’s Manual 12/20/13

8-9

Page 69

Contour Digitize

(F3 from Digitize Menu)

Contour Digitize Run Setup

To set up a digitizing run, jog the probe tip to the center of the part and hit F1 - Center to assign that as your center point.

Select CAM for a true CAM shape contour, or Wall for irregular shapes for wall following. Enter the rest of the parameters for the part and digitizing job as shown below.

Jog the probe to a starting point and press CYCLE START. The control will move the probe toward the center line in the +/- X direction until it comes into contact with the part. At each point of contact, the X and Y coordinates will be recorded in the data file.

The probe will continue around the contour until it returns to the starting point to complete the cycle. Based on the starting point, and the first point of contact, the digitize software will determine if the contour is internal or external.

Important note: When probing an external contour, make sure the probe comes in contact with part on the first move. If it doesn’t, the software will compensate to the outside of the part as if it were an internal contour causing your part to come out larger than you want it to be.

M-Series Operator’s Manual 12/20/13

8-10

Page 70

Contour Digitize Parameters

Copy Type: Toggle between CAM or Wall. Use CAM for regular shapes (no extreme direction changes) and use Wall following for contours with irregular shapes. See example below.

X Patch Length: The length of the contour to be digitized, along the X-axis.

Y Patch Width: The width of the contour to be digitized, along the Y-axis.

Axis Step Over: The distance to pull back away from the surface in the X and/or Y direction. A larger value should be used for a rough digitize along the Y-axis. This distance should be a positive incremental value.

Digitize File Name: The base name of the file in which the digitize data is stored. The file has an extension of .cam for CNC replay and is stored in the c:\cncm\ncfiles directory.

Plunge Rate: The feedrate the Z axis plunges between successive depth passes.

Z Surface Height: Surface height of material for reproduction of digitized parts.

Z Clearance: Clearance to rapid to above surface of part during replay.

Z Depth: Depth of the part as measured from the surface height.

Z Depth Increment: Depth of cut for each Z step of the part.

Probe Diameter: Diameter of probe tip used to digitize the part.

M-Series Operator’s Manual 12/20/13

8-11

Page 71

Contour Digitize Notes

Contour digitizing creates an M&G code file with a .cam extension. The structure of the .cam file starts with a header of comments indicating some of the parameters used when digitizing the contour. Next is the contour itself, which is outputted as a subprogram. The M&G codes are preceded by an O9800 (start of subprogram) and followed by an M99 (end of subprogram). The end of the .cam file contains the initial positioning moves and a call to the contour subprogram (G65 P9800).

Probing direction: When starting the digitizing cycle, choose a starting point where the X travel will contact a point on the cam on the Y axis. The probe tip will move toward the center line in the X direction until it contacts the cam, then will move either clockwise or counterclockwise around the cam, depending on which quadrant you started the cycle (see Table 1).

Table 1 – Probe direction by starting quadrant

X Y Probe travels

- - CW

- + CCW + + CW + - CCW

- 0 CW + 0 CCW

If the probe bypasses a contact point on the Y axis, it will continue moving in the X direction across the center line until it reaches the patch length limit and faults out.

Canceling a job: Unlike grid or radial digitizing if you cancel a contour operation before it is completed you will not be able to restart the contour at the point of interruption to continue the cycle. You will need to start over.

Before running a job: Before running a job created by contour digitizing, you will need to add some information to the file to define any required tool change, cutter compensation and height offset commands.

1. Do a search in the G code for the phrase “Add Comp Here.”

2. Refer to the descriptions of G40, G41 and G42 in Chapter 12.

3. Add the proper G code to the file after the “Add Comp Here” prompt.

4. Save the file, and run your job.

M-Series Operator’s Manual 12/20/13

8-12

Page 72

Wall Following Digitizing

(F8 from Digitize Menu)

Setting up a Wall Following Digitizing Run

To set up a digitize run, edit the parameters shown. Jog the probe tip to the XY starting location (inside or outside of the part to be digitized), and then jog Z to the level of the first digitize pass. Press CYCLE START to start the digitize run.

Wall Following Digitizing Parameters

Probe Tool Number: The tool number of the probe.

Z Patch Distance: The total Z distance to digitize, incremental from the first pass. Entering a negative value will cause the routine to step down in the Z. Entering a positive value will cause the routine to step up in the Z.

Z Step: The Z amount to step down per pass.

Stepover: The distance between the digitized points.

Digitize File Name: The base name of the output file in which the digitize data is stored. An extension of .dig will automatically be appended to the name for replay as a CNC job.

Approach: The direction of the first digitizing move.

Inside/Outside: Starting location of the probe; inside the part or outside.

M-Series Operator’s Manual 12/20/13

8-13

Page 73

Cut Feedrate: The replay feedrate. This is the feedrate that will be output to the file specified by the Digitize File Name above. This will cause the digitized data to be replayed at this specifed feedrate when the output data is run as a CNC job.

Cut Direction: The Clockwise or Counter Clockwise direction of the output data. This also defines the direction of digitze.

Wall Following Digitizing Notes

The output data is uncompensated. Therefore the resultant output data points will be offset by the probe tip’s radius amount. If you want to run this data as a CNC job and actually do cutting, you must use a cutter that is the same shape and diameter as the probe tip. An alternative to this is to use a CAD/CAM software package to remove the probe tip offset and to apply the desired compensation.

M-Series Operator’s Manual 12/20/13

8-14

Page 74

Dig to CAD

(F6 from Digitize Menu)

The Dig to CAD feature of the CNC software is used to export digitized files for use with CAD/CAM software. The digitized files are converted to point cloud data that is easily readable by most CAD/CAM systems. Digitized files have either a .DIG or .DIG5 extension. Files with the extension .DIG are created from the grid or wall following digitizing routines, while .DIG5 files are created from 5-axis digitizing toolpaths. The resulting point cloud data files will have the same file name as the .DIG and .DIG5 files they were created from, only they will have a .TXT extension. These files can then be imported into any CAD/CAM software or viewed with a simple text editor.

In the case of 5-axis CNC controls, where the 4th and 5th axes are rotary axes, parameters 116-119 are used in conjunction with Dig to CAD to properly position the collected data (see Chapter 14 for more information on these parameters).

M-Series Operator’s Manual 12/20/13

8-15

Page 75

Converting Digitized Data

To export digitized data, first select the files you wish to convert by highlighting the files with the arrow keys and using either F1-Toggle or the Space bar to select the files. When a file has been selected an asterisk (*) will appear to the left of the filename. Once you have selected all the files you wish to convert press F10-Accept.

To convert the files and save them in the same directory as the digitized files press Y. To save the files in a different location such as a floppy or USB drive press N, navigate to the desired directory using the file menu, and press F10-Accept to convert and save the files in that location.

M-Series Operator’s Manual 12/20/13

8-16

Page 76

Chapter 9

Probing

Attention!! Refer to the Probe Parameters sections at the end of this chapter before using any

probe.

Part Setup with Probing

Single axis, single surface probing is available on the Set Part 0/Position screen using the F4 - Auto key. This

allows you to probe various surfaces to define the part coordinate system. Multi-axis and multi-surface probing cycles are available on a separate screen, accessible from Set Part 0/Position with the F5 - Probe key or from F4 - Probe in the digitize screen. These allow you to locate the center points and corners of differently shaped parts.

Brushless motor note: If you experience excessive vibration on a brushless drive system, use Parameter 10 to select

smooth deceleration in probing moves. See Chapter 14 for more information.

WARNING: Before manually jogging any probe, make sure the machine Feedrate is slow (less than 10

in/min) or damage to the probe may result!

Automatically Setting Part 0

Part zero can be found using the probe. Make sure your probe height and diameter offsets are set for the tool

number you assigned to the probe and that parameter 12 is set to that tool number. The Edge Finder Diameter will be set automatically.

To set part 0 using the probe:

1. Select the current work coordinate system by pressing F6 – Prev WCS or F7 – Next WCS. Then select the axis you want to probe by pressing F1 – Next Axis.

2. Manually jog the probe about 1/2 inches away from the surface you wish to define. Make sure the approach direction to the part is set properly. Probe the selected axis by pressing F4 - Auto. When the surface is found, the control will assume this point to be the new axis 0.

M-Series Operator’s Manual 12/20/13

9-1

Page 77

3. If you want this probed surface to be something different than 0, enter the value by the using arrow keys to

highlight Part Position, and then type in the value and press F10 - Set.

Repeat steps 1-3 to set the remaining axes using the probe. Any previously entered Edge Finder Diameter or Tool

Number value will be discarded.

Finding Center/Corner Points

To enter the Probing Cycles screen, press F5 - Probe from the Set Part 0/Position screen. You can locate the center

of a bore, boss, slot, or web. You can also find an inside corner, outside corner, or a single axis. The corner points don’t even have to be right angles! The Edge Finder Diameter doesn’t need to be entered since these cycles place the probe directly over the center or corner of the part.

Calibrating the Probe Tip Diameter

You can calibrate the probe tip diameter to compensate for pre-travel (the amount that the probe deflects before it

actually trips). Simply enter a probe tip diameter of zero, probe out a precision bore with a known diameter, and enter the difference between the reported bore diameter and the found bore diameter as the actual probe tip diameter.

Probing Cycles

You can enter the Probing Cycles screen from either the Set Part 0/Position screen (F5 - Probe) or the Digitize

menu (F4 - Probe). The Probing Cycles screen is shown below:

The probing cycles will report the location and dimensions, as applicable, of the probed feature in a floating dialog

box. The dimensions are adjusted to compensate for the probe tip diameter, entered in the Offset Library (see Parameter 12). For your convenience, you can edit the probe diameter on this screen, as long as the Tool Number, as set in Parameter 12, is not 0. During the probing cycles, the probe will move at speeds specified in Parameters 14 and 15. Refer to the Probe Parameters section later in this chapter for more information.

M-Series Operator’s Manual 12/20/13

9-2

Page 78

F1 – Bore Press F1 - Bore to enter the Bore screen. A picture similar to the one shown at right will appear,

with instructions. Follow these steps:

1 - Make sure the probe is clear of any obstacles. 2 - Manually jog the probe inside the hole. The probe tip should be just below the top edge of the surface. 3 - Press CYCLE START to start the probing. At the end of probing, the probe will be positioned at the center of the bore, and the X and Y positions will be

shown on the screen.

Press ESC to return to the Set Part 0/Position screen or digitize screen.

F2 – Boss Press F2 - Boss to enter the Boss screen. A picture similar to the following will appear, with

instructions and two input fields. Follow these steps:

1 - Press F1 - Orient to select the orientation of the probe with respect to the Boss. You will see one of the screens

shown below.

2 - Slowly jog the probe to the approximate orientation as shown in the picture. Be sure to give enough space for

the probe tip to clear any obstacles during the jog. 3 - Enter the approximate Boss diameter. 4 - Highlight the Z clearance amount by pressing the down arrow key. Enter approximate distance (in the Z

direction) the probe must move to lift up over the Boss. 5 - Press CYCLE START to start the probing cycle.

If the Z clearance you entered is too small, the probe will stop and show an error message. Correct the problem by

repeating the previous steps. If the approximate diameter you entered is too small, the probe will bounce by 10 percent of its diameter across the top surface until it either finds the correct edge, the additional distance searched is equal to Parameter 16, or a travel limit is reached.

Once the probing cycle is complete, the probe will be positioned at the center of the boss at the Z clearance level

entered. Press ESC to return to the Set Part 0/ Position screen or digitize screen.

M-Series Operator’s Manual 12/20/13

9-3

Page 79

F3 – Slot

instructions:

1 - Press F1 - Orient to select the orientation of the probe with respect to the slot. 2 - Slowly jog the probe to the approximate position shown in the picture. During this jog, make sure you have

enough space between the probe and the part.

3 - Press CYCLE START to begin probing.

Once the cycle is finished, the probe will be located at the center of the slot. Press ESC to return to the Set Part 0 –

Position Screen or digitize screen.

Press F3 - Slot to enter the Slot screen. A picture similar to the ones shown will appear along with

F4 – Web Press F4 - Web to enter the Web screen. A picture similar to the following will appear,

with instructions and two input fields. Follow these steps:

1 - Press F1 - Orient to select the orientation of the probe. You will see one of the screens shown below. 2 - Slowly jog the probe to the approximate position shown in the picture.

During this jog, be sure to give enough space between the probe and the part. 3 - Enter the approximate Web width. 4 - Highlight the Z clearance value using the up or down arrow key. Enter

approximate distance the probe has to travel in order to lift up over the Web. 5 - Press CYCLE START to start the probing cycle. Once the probe has completed its search, it will automatically position to the centerline of the web.

If the Z clearance you entered is too small, the probe will stop and show an error message. Correct the problem by

repeating the previous steps. If the approximate width you entered is too small, the probe will bounce by 10

percent of its width across the top surface until it either finds the correct edge, the additional distance searched is

equal to Parameter 16, or a travel limit is reached.

Once the probing cycle is complete, the probe will be positioned at the center of the web, at the Z clearance level

entered. Press ESC to return to the Set Part 0/ Position screen or digitize screen.

M-Series Operator’s Manual 12/20/13

9-4

Page 80

F5 - In Corner (Inside Corner) Press F5 - In Corner to enter the Inside Corner screen. One of the

pictures will appear with instructions. This cycle is similar to that of a slot cycle; the main difference is that you need to enter a clearance amount.

1 - Press F1 Orient and the screen will cycle through one of the probe orientations shown here. 2 - Enter the clearance Amount. This is an approximate distance (in the Z direction) the probe must move to clear

the corner

3 - If the corner is rounded, jog the probe far enough away for it to miss the curved area during the probing cycle (at

least twice the corner radius).

4 - Press CYCLE START to start the probing cycle.

At the end of the probing cycle, the probe will be positioned above the corner at the Z clearance level entered. Press

ESC to return to the Set Part 0/ Position screen or digitize screen.

F6 - Out Corner (Outside Corner) Press F6 – Out Corner to enter the Outside Corner screen. A picture

similar to the following will appear, with instructions and two input fields.

Follow these steps: 1 - Press F1 - Orient to select the orientation of the probe with respect to the Corner. You will see one of the

pictures shown.

2 - Press F2 - Side to select which side of the corner the probe will be positioned near. You will see the screen

change.

3 - Slowly jog the probe to the approximate position as shown in the picture. Be sure to give enough probe

clearance.

4 - Select the Z clearance field using the arrow keys. Enter the approximate distance the probe has to travel in order

to lift up over the corner.

5 - Select the Distance to Corner amount using the up or down arrow keys. Enter the approximate distance from the

corner the probe is along the X or Y axis.

6 - Press CYCLE START to start the probing cycle.

Once the probe has completed its search, it will be positioned above the corner at the Z clearance you specified.

Press ESC to return to the Set Part 0/ Position screen or digitize screen.

M-Series Operator’s Manual 12/20/13

9-5

Page 81

F7 - 1 Axis (Single Axis) Press F7 - 1 Axis to enter the Single Axis screen. Follow these steps:

1 - Press F1 - Orient to select the orientation of the probe. You will see one of the screens shown below. 2 - Slowly jog the probe to the approximate position as shown in the picture. Be sure to give enough probe

clearance. 3 - Press CYCLE START to start the probing cycle.

Once the probing cycle is complete, the probe will move away from the surface by the amount in Parameter 13. The

probed position will be shown on screen. Press ESC to return to the Set Part 0/ Position screen or digitize screen.

F8 – Angle – Use this feature to measure an angle from based on 2 probed points.

Follow these steps:

1 - Press F1 - Orient to select how the angle is to be measured. 2 - Slowly jog the probe to the first position as shown in the picture. Be sure to give enough probe clearance. 3 - Select Auto or Jog between points. 4 - Enter the distance to second point. 5 - Enter a clearance amount away from the surface. 6 - Press CYCLE START to start the probing cycle.

M-Series Operator’s Manual 12/20/13

9-6

Page 82

Probe / TT-1 Parameters

Various probing parameters can be set on the Machine Parameters screen (see Chapter 14). Make sure you enter

these parameters before you begin using the probe and/or TT-1. If these parameters are not entered properly, damage to the probe or TT-1 may result.

Probe Type (Parameter 155) – This specifies the probe type being used. This needs to be set to 0 if you are using

a standard Mechanical probe.

Probe PLC Input Number and Contact State (Parameter 11) - A single value, +/-1 through 240. A positive

number indicates Closed on contact; a negative number indicates Open on contact.

TT1 PLC input number (Parameter 44) - This parameter is the input number that the TT1 is wired into on the

PLC. If a shared PLC input is used for both the TT1 and the probe, then the value can be left at zero or set to the same value as parameter 11.

Probe Tool Number (Parameter 12) - A single value, 0 through 200, used to look up the length offset and tip

diameter of the probe in the Offset Library.

Recovery Distance* (Parameter 13) – The additional distance the probe moves off of a surface after contact is

broken, before attempting to traverse parallel to the surface.

Fast Probing Rate* (Parameter 14) - Used for positioning moves and initial surface detection, this parameter is

determined by machine response and permitted probe deflection as well as desired tolerance. The default setting is 25 inches/min.

Slow Probing Rate* (Parameter 15) - Used for final measuring moves, this parameter is determined by a

speed/accuracy tradeoff. The default setting is 3.5 inches/min.

Maximum Probing Distance (Parameter 16) - The maximum distance that a probing cycle "searches" for a

surface in a given direction if no travel limits have been entered. The default is 10 inches. A larger value should be entered for the hole and slot cycles if you are measuring very large features.

Detector Location Return Point (Parameter 17) - A Zero (0) indicates that tool measurement will take place at

the current position, a 1 or 2 indicates the number of the G30 reference point to use which specifies the X, Y location of the TT1 (WCS Configuration).

*Mechanical type probe only. Please see the DSP type probe section below for differences.

M-Series Operator’s Manual 12/20/13

9-7

Page 83

DSP Probe Parameters

When using a DSP type probe (such as DP-4D), a few of the probing parameters have a slightly different behavior

than described above. These differences are noted below:

Probe Type (Parameter 155) – This specifies the probe type being used. This needs to be set to 1 for a DP-4D

probe or set to 2 for a DP-7 probe.

Repeatability tolerance for probing and radial digitizing (Parameter 151) – used for DP-4 probes. Must be set

to 0 for DSP probes.

Grid digitize prediction minimum Z pullback (Parameter 121) – set to 0.035 for DSP use.

Recovery Distance (Parameter 13) – Works as described above but additionally it used as the distance to retract

for a retry after a failed window (does not apply to M115/116/125/126 moves) (Default for DSP is 0.05). Note: If

probing small bores this parameter may need to be reduced accordingly. Fast Probing Rate (Parameter 14) – When using a DSP type probe, this is actually the rate at which the probe

will move “in-between” actual probing moves. For instance, if you were probing a boss, this is the rate at which

the probe will travel for the following moves:

1. When retracting from the surface after a point has been probed.

2. When retracting to the Z clearance position.

3. Rate at which it will traverse across the diameter of the boss at the Z clearance height.

4. Plunge rate to get to probing depth.

Note: When measuring a TOOL with the TT1, the behavior is identical to that listed above.

Slow Probing Rate (Parameter 15) – Used only when measuring a TOOL with the TT-1.

Additional Probe Parameters for DP-7

For the DP-7 probe (parameter 155 = 2), the following additional parameters are utilized:

DP-7 Pullback Distance (Parameter 392) – This sets the distance the probe moves off from the surface after a

probing move.

DP-7 Pullback Feedrate (Parameter 393) – This sets the feedrate for the pullback move. DP-7 Measuring Feedrate (Parameter 394) – This sets the feedrate for the slow measuring move.

M-Series Operator’s Manual 12/20/13

9-8

Page 84

Chapter 10

Intercon Mill

Intercon Mill Intercon Mill

Intercon Mill

Current Part: Flange.icn

Current Part: Flange.icn Current Part: Flange.icn

Current Part: Flange.icn

FFFF

1111

FFFF

2222

Copy

CopyCopy

Copy

FFFF

7777

FFFF

5555

FFFF

3333

FFFF

4444

FFFF

6666

FFFF

8888

FFFF

1010

FFFF

9999

;Motor Flange

;Motor Flange;Motor Flange

;Motor Flange

Home

Home Home

Home

0.0000

0.00000.0000

0.0000

0.00000.0000

0.0000

0001

00010001

0001

Operation End

Operation End Operation End

Operation End

Status

StatusStatus

Status

Intercon Software

Introduction

Intercon (Interactive Conversational) software allows you to quickly create a part program right at the control without having to be a G-code expert. Intercon will prompt you to enter values from your print that describes the geometry of the part. Intercon will display graphics of the part as you are creating it, helping you quickly proceed through part programming. Intercon can then generate a G-code program from the geometric information you have entered.

You can purchase an offline version of the Intercon software for use on your desktop PC. You will need to purchase a hardware key, which will allow the offline version to run. Simply plug the key into the computer, install the required drivers, and run it.

Intercon Main Screen

When you access Intercon through the F5 - CAM option in the CNC software Main screen, the part program will be displayed if the current job loaded in CNC software had an associated Intercon program. If the job file in the CNC software did not have an associated Intercon program, the F1 - File menu will be displayed to load or create a file.

Modify

ModifyModify

0.0000

0.00000.0000

1.0607

1.06071.0607

3.2500

3.25003.2500

3.2500

3.25003.2500

Insert

InsertInsert

0.1000

0.10000.1000

0.1000

0.10000.1000

0.1000

0.10000.1000 Home

Home

Home Home

Paste

PastePaste

Copy

CopyCopy

Menus..

Menus..Menus..

Graph

GraphGraph

Setup

SetupSetup

Post

PostPost

0.0000

0.00000.0000

1.6070

1.60701.6070

4.1250

4.12504.1250

4.1250

4.12504.1250

Cut

CutCut

# Type X Y Z

# Type X Y Z # Type X Y Z

0002

00020002 0003

0003

00030003 0004

0004

00040004 0005

0005

00050005 0006

0006

00060006

Tool #1

Tool #1Tool #1 Circ Poc

Circ Poc

Circ PocCirc Poc Drill BHC

Drill BHC

Drill BHCDrill BHC Frame

Frame

FrameFrame End Prog

End Prog

End ProgEnd Prog

File

FileFile

When the part program is displayed, different operations can be navigated and highlighted for additional actions by using the arrow keys, and the HOME, END, PAGE UP and PAGE DOWN keys.

M-Series Operator’s Manual 12/20/2013 10-1

Page 85

File Menu (Intercon Main Screen ► F1 – File)

Intercon Mill

Intercon Mill Intercon Mill

Intercon Mill

Current Part: Flange.icn

Current Part: Flange.icn Current Part: Flange.icn

Current Part: Flange.icn

FFFF

1111

FFFF

2222

FFFF

5555

FFFF

3333

As As

F4 F4

Details

DetailsDetails

Details

FFFF

9999

Intercon File Menu

Intercon File Menu Intercon File Menu

Intercon File Menu

[ a:

[ a:[ a:

[ a:

\\\\

]]]]

Drive

DriveDrive

Drive

Sandisk

SandiskSandisk

Sandisk

File Programmer Description Date Modified

File Programmer Description Date Modified File Programmer Description Date Modified

File Programmer Description Date Modified

John Q. Public

John Q. PublicJohn Q. Public

John Q. Public

0606

----

Oct

OctOct

Oct

----

2006

20062006

2006

Directory: c:

Directory: c:Directory: c:

Directory: c:

\\\\

intercon

intercon intercon

intercon

Floppy

Floppy Floppy

Floppy

FFFF

2222

Details

DetailsDetails

Details

FFFF

3333

Show

ShowShow

Show

FFFF

4444

Date/

Date/Date/

Date/

FFFF

5555

FFFF

6666

Help

HelpHelp

Help

FFFF

7777

FFFF

9999

F1F1

0000

G code

G code G code

G code

F1F1

Load file from CNC hard drive

Load file from CNC hard driveLoad file from CNC hard drive

Load file from CNC hard drive

c:c:

\\\\

intercon

interconintercon

intercon

Use arrow keys to select file to load and press F10 to Accept.

Use arrow keys to select file to load and press F10 to Accept.Use arrow keys to select file to load and press F10 to Accept.

Use arrow keys to select file to load and press F10 to Accept.

Job

Job Job

Job

toto

load? bracket.cnc

load? bracket.cnc load? bracket.cnc

load? bracket.cnc

[..]

[..][..]

[..]

Parent directory

Parent directoryParent directory

Parent directory

File Programmer

File Programmer File Programmer

File Programmer

Description Date Modified

Description Date Modified Description Date Modified

Description Date Modified

0606

----

Oct

OctOct

Oct

----

2006

20062006

2006

F1 – File

Choosing F1 - File will display the screen below. Intercon stores part programs with an extension of

.icn. For example, if you choose to name your new part program flange, Intercon will save the program as flange.icn. ICN files are only readable by Intercon.

[ c:

[ c:\\\\]]]]

[ c:[ c: [ d:

[ d:\\\\]]]]

[ d:[ d: [ j:

[ j:\\\\]]]]

[ j:[ j: [..]

[..]

[..][..] flange

flange

flangeflange helix

helix

helixhelix irreg

irreg

irregirreg lineclr

lineclr

lineclrlineclr thread

thread

threadthread __oscp__

__oscp__

__oscp____oscp__ __osda__

__osda__

__osda____osda__ __osdb__

__osdb__

__osdb____osdb__ __osdr__

__osdr__

__osdr____osdr__ __osfa__

__osfa__

__osfa____osfa__ __osfr__

__osfr__

__osfr____osfr__ __osrp__

__osrp__

__osrp____osrp__

John Q. Pu

John Q. Public

John Q. PuJohn Q. Pu John Q. Public

John Q. Public

John Q. PublicJohn Q. Public

---John Q. Public

John Q. Public

John Q. PublicJohn Q. Public One Shot Circ Pocket

One Shot Circ Pocket

One Shot Circ PocketOne Shot Circ Pocket One Shot Drill Array

One Shot Drill Array

One Shot Drill ArrayOne Shot Drill Array One Shot Drill BHC

One Shot Drill BHC

One Shot Drill BHCOne Shot Drill BHC One Shot Drill Cycle

One Shot Drill Cycle

One Shot Drill CycleOne Shot Drill Cycle One Shot Face

One Shot Face

One Shot FaceOne Shot Face One Shot Frame

One Shot Frame

One Shot FrameOne Shot Frame One Shot Rect Pocket

One Shot Rect Pocket

One Shot Rect PocketOne Shot Rect Pocket

blic

blicblic

Drive

DriveDrive Drive

Drive

DriveDrive Drive

Drive

DriveDrive Parent directory

Parent directory

Parent directoryParent directory Demo Flange Part

Demo Flange Part

Demo Flange PartDemo Flange Part Demo Helix Part

Demo Helix Part

Demo Helix PartDemo Helix Part Demo Pocket Cleanout

Demo Pocket Cleanout

Demo Pocket CleanoutDemo Pocket Cleanout

---Demo Thread

Demo Thread

Demo ThreadDemo Thread * DO NOT MODIFY *

* DO NOT MODIFY *

* DO NOT MODIFY * * DO NOT MODIFY *

* DO NOT MODIFY *

* DO NOT MODIFY * * DO NOT MODIFY *

* DO NOT MODIFY *

* DO NOT MODIFY * * DO NOT MODIFY *

* DO NOT MODIFY *

* DO NOT MODIFY * * DO NOT MODIFY *

* DO NOT MODIFY *

* DO NOT MODIFY * * DO NOT MODIFY *

* DO N

* DO NOT MODIFY *

* DO N * DO N

* DO NOT MODIFY *

* DO NOT MODIFY * * DO NOT MODIFY *

OT MODIFY *

OT MODIFY *OT MODIFY *

06----Oct

Oct----2006

0606

OctOct

06----Oct

Oct----2006

0606

OctOct

19----Nov

Nov----2006

1919

NovNov

06----Oct

Oct----2006

0606

OctOct

06----Oct

Oct----2006

0606

OctOct

06----Oct

Oct----2006

0606

OctOct

06----Oct

Oct----2006

0606

OctOct

06----Oct

Oct----2006

0606

OctOct

06----Oct

Oct----2006

0606

OctOct

06----Oct

Oct----2006

0606

OctOct

06----Oct

Oct----2006

0606

OctOct

2006

20062006 2006

20062006

2006

20062006

2006

20062006 2006

20062006

New

Load

NewNew

Load

LoadLoad

Save

SaveSave

Save

Save Save

Delete

DeleteDelete

On/Off

On/OffOn/Off

F1 – File ► F1 – New

To program a new part, choose F1 – New. A prompt will be displayed where the name

of the new program can be typed, followed by the F10 - Accept or ENTER key to accept the new name can be entered. You can enter who the programmer is, a program description, the units of measure and the date.

Load Menu (Intercon Main Screen ► F1 – File ► F2 – Load)

F1 – File ► F2 – Load

M-Series Operator’s Manual 12/20/2013 10-2

flange

flangeflange

helix

helixhelix

irreg

irregirreg

thread

threadthread

__oscp__

__oscp____oscp__

__osda__

__osda____osda__

_____osdb__

_osdb__

_osdb___osdb__

/ICN

/ICN/ICN

////USB/

When you press F2 - Load, the screen below is displayed. (Shown with details “ON”)

John Q. Public

USB/LAN

LAN

USB/USB/

LANLAN

John Q. PublicJohn Q. Public John Q. Public

John Q. Public

John Q. PublicJohn Q. Public John Q. Public

John Q. Public

John Q. PublicJohn Q. Public One Shot Circ Pocket

One Shot Circ Pocket

One Shot Circ PocketOne Shot Circ Pocket One Shot Drill Array

One Shot Drill Array

One Shot Drill ArrayOne Shot Drill Array One Shot Drill BHC

One Shot Drill BHC

One Shot Drill BHCOne Shot Drill BHC One Shot Drill Cycle

One Shot Drill Cycle

One Shot Drill CycleOne Shot Drill Cycle

On/Off

On/OffOn/Off

Recent

RecentRecent

Demo Flange Part

Demo Flange PartDemo Flange Part

Demo Helix Part

Demo Helix PartDemo Helix Part

Demo Pocket Cleanout

Demo Pocket CleanoutDemo Pocket Cleanout

Demo Thread

Demo ThreadDemo Thread

* DO NOT MODIFY *

* DO NOT MODIFY * * DO NOT MODIFY *

* DO NOT MODIFY *

* DO NOT MODIFY * * DO NOT MODIFY *

* DO NOT MODIFY *

* DO NOT MODIFY * * DO NOT MODIFY *

Edit

Alpha

AlphaAlpha

EditEdit

On////Off

Off

OnOn

OffOff

06----Oct

0606 00006666----Oct 19

19----Nov

1919 06

06----Oct

0606 06

06----Oct

0606 06

06----Oct

0606 06

06----Oct

0606

Advanced

Graph

Graph Graph

AdvancedAdvanced

Oct----2006

2006

OctOct

20062006

Oct----2006

2006

OctOct

20062006

Nov----2006

2006

NovNov

20062006

Oct----2006

2006

OctOct

20062006

Oct----2006

2006

OctOct

20062006

Oct----2006

2006

OctOct

20062006

Oct----2006

2006

OctOct

20062006

AcceptAccept

Page 86

To navigate the files in the load menu, use the arrow keys to move the cursor around and highlight the file to be loaded. The HOME, END, PAGE UP and PAGE DOWN keys can be used to navigate the list of files. Names that are bracketed, for example [..], are the names of directories in the current directory, which is displayed at the top of the screen.

It is also possible to start typing the name of the program to be loaded. When typing has started, the characters appear in the “File to load:” prompt above the function keys. Different drives and directories can be accessed by typing in the path at the “File to load:” prompt, or by pressing F10 or ENTER on a bracketed directory name. When loading a new file, a prompt will be displayed asking whether to save the existing file if there was one.

Additional Load Menu options are detailed below:

F1 – G code/ICN Allows user to toggle the view between the Intercon files present in either c:\intercon or c:\cncm\ncfiles.

F2 – Floppy USB/LAN Provides options for loading Intercon files from USB devices, floppy and LAN drives. F3 – Details On/Off The F3-Details On/Off option changes the format of the display such that each file or directory

is on a separate line and there are columns displayed for Programmer, Description, and Date Modified, i.e., the information that is contained in the program header operation.

F4 – Show recent Use the F4–Show Recent option to show the 15 most recently loaded Intercon and g-code files. It is important to remember that even though g-code files are displayed on this screen, ONLY Intercon files should be loaded from this screen. WARNING!!! Attempting to load a g-code file from the “Show Recent” screen will cause an error which will discard the current Intercon program. All unsaved changes will be lost. If you should accidently load a g-code file, press escape to return to the main Intercon menu.

F5 – Date/Alpha Use F5-Date/Alpha to view files either alphabetically or by date modified. By default, programs are listed in ascending alphabetical order.

F6 – Edit Opens the selected file in Intercon for editing. F7 – Help On/Off Displays on screen help for the load menus.

F8 – Graph Graphs the selected file.

F9 – Advanced Displays file menu in a comprehensive “all in one” format similar to Windows Explorer

File Menu (Intercon Main Screen ► F1 – File, continued from pg 10-2)

F1 – File ► F3 – Save

under the specified name.

F1 – File ► F4 - Save As

new name into the “Save part as:” prompt that appears above the function keys. If the new name already exists, a prompt will be displayed as a warning and will give the option to overwrite the existing file or return to enter a different name.

F1 – File ► F5 – Delete

as in the F2 - Load option where you can be to navigate the files. A yes/no prompt will appear after accepting a file for deletion for final confirmation.

M-Series Operator’s Manual 12/20/2013 10-3

Press F3 - Save to save the current part program. The current program will be saved

Press F4 – Save As to save the current program with a different name. Type the

Press F5 - Delete to delete a file. After F5 - Delete is pressed, the screen will appear

Page 87

F1 – File ► F9 - Details on/off

file or directory is on a separate line and there are columns displayed for Programmer, Description, and Date Modified, i.e., the information that is contained in the program header operation.

The F9 - Details On/Off changes the format of the display such that each

Intercon Main Screen (continued from pg 10-1)

F2 – Modify

to be modified. When an operation is modified, the fields for that operation are displayed on the right hand side. When modifying an operation, the PAGE UP and PAGE DOWN keys can be used to move up and down through the Intercon operations listed on the left hand side of the screen.

F3 – Insert

unless the highlighted operation is the first operation in which case the inserted operation will be inserted as the second operation. For more information on the operations see Insert Operations later in this chapter.

F4 – Cut

cut is placed onto the clipboard stack.

F5 – Paste

current program line that is before the highlighted operation. The number of operations that are currently in the clipboard stack are indicated by the number in the Paste key. As long as you stay in Intercon, the clipboard stack will remain intact. You may cut and copy operations from one program and paste them into a different program.

F6 – Copy

cursor to the next operation.

F7 – Copy Menus…

F1 - Copy Menu Allows a range of operations to be copied. Specify the Start Block, End Block, and Destination in the prompts that appear in the Copy Menu. The range of operations is copied into a location that precedes the destination block. F2 - Move Menu Allows a range of operations to be moved. Specify the Start Block, End Block, and Destination in the prompts that appear in the Move Menu. The range of operations is moved into a location that precedes the destination block. F9 - Clear Clipbrd Removes all operations in the clipboard stack.

F8 – Graph

produced if the current program were translated into G-codes and graphed from the CNC software. Canned drilling cycles are shown in gray. Rapid traverse movements are shown in red. Feedrate movements are shown in yellow and cutter compensated moves are in gray.

Choosing F2 - Modify from the Intercon main menu will allow the currently highlighted operation

Choosing F3 - Insert will insert a new operation before the operation that is currently highlighted,

Choosing F4 - Cut will cut (remove) the highlighted operation from the program. The operation that is

Choosing F5-Paste will paste the last operation that was cut or copied into the clipboard stack into the

Choosing F6 - Copy will copy the highlighted operation into the clipboard stack and advance the

Choosing F7 - Copy Menus… will display these additional options:

Choosing F8 - Graph will graph the current program. The graph is the same as what would be

M-Series Operator’s Manual 12/20/2013 10-4

Page 88

F9 – Setup

appears as below.

Choosing F9 - Setup will display the Setup menu where certain options can be set. The Setup menu

Use the up and down arrow keys to move. Clearance Amount, Spindle/Coolant Delay, and Corner Feedrate Override require a value to be typed in. The other fields have fixed values that may be toggled by using the F1 - Toggle key.

Comment Generation: When this field is set to Enabled, Intercon will put a comment describing the operation type before each block. Disabling Comment Generation will make the CNC files generated by Intercon smaller. Clearance Amount: This is the distance that Intercon raises the Z-axis above the programmed surface height in pockets, facing and frame mills when traveling across the work piece. Spindle/Coolant Delay: Set this delay to the time in seconds you want Intercon to wait for the spindle to get up to speed and the coolant to begin flowing. Corner Feedrate Override: This is the percent feedrate that will be used in the corners of rectangular pockets and inside frame mills. The default value is 50%. Modal Operations: These options specify whether to automatically insert the same operation after the first has been accepted. Once modal insert mode has begun, press ESC to insert a different operation. Rotary 4th Axis: This option specifies whether or not 4th axis movement fields appear in Linear and Rapid moves and whether or not the Intercon program will post 4th axis movement. This option affects the value in the 4th axis configuration only (parameter 94). Note that although Intercon is restricted to working with 1 rotary axis at a time, it can be directed to utilize the 5th axis as its rotary axis instead of the 4th. To make Intercon to utilize the 5th axis as its rotary axis instead of the 4th axis, the 4th axis configuration (parameter 94) must have its rotary property turned off (bit 0 = 0) and the 5th axis configuration (parameter 166) must have its rotary property turned on (bit 0 = 1). See chapter 14 for details about parameters 94 and 166. DRO Units: Specifies the Units used for the DRO. It affects the corresponding field in the Control Configuration. Machine Units: Specifies the Units used for machining. It affects the corresponding field in the Control Configuration of the CNC software. The posted G-code will contain a G20 for Inches mode and a G21 for Metric mode. Help Icons always on: Toggle between yes or no. Selecting “yes” means that help information will always be displayed when editing operations. “No” means that you will have to press a key to get help. Whether set to “yes” or “no”, the help screens can always be toggled on or off by pressing the F5 - Help key when editing an operation. Cutter Comp Look-ahead: This sets the number of segments that can be parsed ahead when Cutter Comp is turned on.

F10 – Post

into G-codes. When the posting process is completed, Intercon is exited. The Intercon program is also saved as part of the posting.

Choosing F10 - Post will post the current program. Posting is the process of converting the operations

M-Series Operator’s Manual 12/20/2013 10-5

Page 89

Insert Operation (Intercon Main Screen ► F3 – Insert)

When you press F3 - Insert, or when you choose New Part from the Main Screen, you will see the Insert screen:

The new operation will be inserted right before the currently highlighted one. The operation types that you can insert are listed across the bottom of the screen.

M-Series Operator’s Manual 12/20/2013 10-6

Page 90

F1 - Rapid Traverse

the following screen:

Press F1 - Rapid from the Insert Operation screen to insert a Rapid Traverse. You may see

End: When you first access the rapid traverse screen, the cursor will be highlighting the first field, End X. This is the X coordinate of where the cutter will be after the rapid traverse has been completed. Similarly, Y and Z represent the coordinates of the cutter after the rapid traverse is completed. The angle and length fields will be computed if you choose to enter the end point of the move.

Angle: The destination may also be specified in terms of a counterclockwise angle from the three o'clock position. When combined with a length for the current move, the corresponding X and Y coordinates for the destination will be calculated and placed in the correct fields. The Z destination will remain unchanged, however.

Length: The length of the rapid traversal. When combined with the angle of the current move, the corresponding X and Y coordinates for the destination will be calculated and placed in the correct fields. The Z destination will remain unchanged, however.

The F1 – Abs/Inc key toggles between incremental and absolute positioning modes in any of the fields where a positional dimension is needed. For example: X, Y, or Z-axis dimensions can all be in incremental or absolute coordinates, or a mixture of both. The length and angle fields cannot be incremental. These fields are absolute values.

The F2 - Z Home key may be used on the Z destination field to tie the ending Z coordinate to the Z home position. This means that no matter what you’re Z home value is at the time that you run your program, the final Z position will be the Z home position.

When you are finished entering all of the dimensions for the rapid move, press F10 - Accept to accept the operation and return to the Insert Operation screen.

NOTE: When making rapid moves, if a Z destination higher than the current cutter position is specified, the cutter will first be raised to the destination Z position, and then move linearly in X and Y to arrive at the destination. If a Z destination lower than the current cutter position is specified, the cutter will move linearly in X and Y first and then plunge Z to the destination Z position.

NOTE: The Rapid traverse operation can have rotary fields, if you have a rotary fourth axis. The rotary field descriptions are the same as that of the Linear Mill operation.

M-Series Operator’s Manual 12/20/2013 10-7

Page 91

F2 - Linear Mill

If you press F2 - Linear from the Insert Operation screen, the following screen appears:

The numbers in the different fields on the screen correspond to the following Linear Mill example shown here graphically:

End: When you first access the linear mill screen, the cursor will be highlighting the first field, End X. This is the X coordinate of where the cutter will be after the linear move has been completed. Similarly, Y and Z represent the coordinates of the cutter after the linear move is completed. The angle and length fields will be computed if you choose to enter the end point of the move.

Length: The length of the linear mill. When combined with the angle of the current move, the corresponding X and Y coordinates for the destination will be calculated and placed in the correct fields. The Z destination will remain unchanged, however.

Connect Radius: If you are performing two linear mill operations and you wish to have a rounded 'corner' between them instead of a sharp peak, you may enter the radius of the 'corner' and Intercon will insert an arc between the linear mill operations. This connect radius also works for blending a line into an arc operation.

Feedrate: Speed at which the cutter moves.

M-Series Operator’s Manual 12/20/2013 10-8

Page 92

The feedrate can be toggled to modal, fixed, or slave. This is indicated by the symbol beside the feedrate field. If the feedrate is modal then it will have the “M” symbol or if it is fixed it will have the “F” symbol shown below. The slave feedrate has no symbol and is set to the last modal feedrate set in the program, when the modal feedrate changes all the following slave feedrates change until the next modal feedrate is encountered.

If you have a fourth axis installed and it is rotary, additional fields are shown for Linear Mill operations after the feedrate field.

Degrees: The number of degrees you want to move the rotary axis. This value can be positive or negative and the movement of the rotary axis will depend on the orientation of the axis.

Minutes: The number of minutes you want to move the rotary axis. Values for this field are between 0 and 59.

Seconds: The number of seconds you want to move the rotary axis. Values for this field are between 0 and 59.

Decimal degrees: This is another method of entering the number of degrees. If you choose to enter the movement of the rotary axis with the fields listed above, the value of this field will be calculated automatically. If you choose to enter the number of degrees with this field or make changes to it, then the degrees, minutes and seconds will be calculated or changed automatically. Values for this field can be positive or negative.

Rotary movement defaults to zero degrees, incremental. To enter an absolute (rather than incremental) rotary position, you must press F1 - Abs/Inc to toggle to absolute.

M-Series Operator’s Manual 12/20/2013 10-9

Page 93

F3 - Arc Mill

If you press F3 - Arc for Arc Mill from the Insert Operation screen, the following screen appears:

The numbers in the different fields on the screen correspond to the following Arc Mill example shown here graphically:

Operation Type: There are four ways to specify your ARC: using an endpoint and a radius (EP&R), using a center point and an angle (CP&A), using a center point and an end point (CP&EP), or using a mid-point and an end point (3Point). The Three Point arc is designed to be used in conjunction with Teach Mode. When specifying a particular kind of arc, you will not be able to modify certain fields. For example, if you are specifying an endpoint and a radius, you will not be able to modify the mid point, center point and angle fields. This is because Intercon calculates the correct values for these fields.

Mid: The X, Y, and Z coordinates of a point on the arc path somewhere between the start point and end point of the arc. You will be able to modify this field only when specifying a Three Point arc. Also, the coordinate that does not lie in the plane of the arc cannot be edited; it is automatically calculated.

End: The X, Y and Z coordinates of where the cutter will be once the arc move is complete. You will not be able to edit this field if you are specifying a center point and angle (CP&A) arc.

Center: This is the X, Y and Z position of the center of the arc. You will not be able to edit this field if you are specifying an end point and radius (EP&R) arc or a Three Point arc. Also, the coordinate that does not lie in the plane of the arc cannot be edited; it is automatically carried forward from the last operation.

M-Series Operator’s Manual 12/20/2013 10-10

Page 94

Angle: Number of degrees through which the cutter will travel. This value must lie between 0 and 360 degrees. You will be able to edit this field only if you are specifying a center point and angle (CP&A) arc.

Radius: Distance from the center of the arc to its edge. This value must be greater than 0. You will only be able to edit this value if you are specifying an end point and radius (EP&R) arc.

Plane: This determines whether the arc is to be milled in the XY-, ZX- or YZ-plane. If any of the Z coordinate values are tied to the Z home position, only XY-plane arcs may be selected.

Direction: Determines whether the arc moves clockwise (CW) or counterclockwise (CCW). Note that the direction of XZ arcs is judged looking Y+ (i.e. from the front of the machine). This is natural, but it is opposite of the way arcs are specified in G codes. Intercon automatically makes this translation when it generates CNC codes.

Connect Radius: This field works like the Linear Mill connect radius. It allows for the blending of an arc into the next line or arc operation.

Feedrate: Speed at which the cutter moves. The feedrate can be toggled to modal, fixed or slave, this is indicated by the symbol beside the feedrate field. If the feedrate is modal then it will have the “M” symbol or if it is fixed it will have the “F” symbol shown below. The slave feedrate has no symbol and is set to the last modal feedrate set in the program, when the modal feedrate changes all the following slave feedrates change until the next modal feedrate is encountered.

Angle <= 180º: For end point and radius (EP&R) arcs, this field determines whether the arc is to be less than (YES) or greater than (NO) 180 degrees.

M-Series Operator’s Manual 12/20/2013 10-11

Page 95

F4 - Tool Functions

When you select the tool functions by pressing F4 - Tool the following screen appears:

The following parameters for this tool change are as follows:

Tool Number: Number of the tool (between 1 and 200) to use. Entering this value pulls the current settings for this tool from the CNC software tool library. You may then edit the length offset, diameter offset and diameter values if you wish to redefine your tool. The length value is not editable.

Description: Description of the tool selected above, from the tool library.

Position: X and Y coordinates for the place at which the tool change will occur. This should be a place at which the current tool can be removed from the quill and the new tool can be inserted.

Tool H Offset: Index in the offset library (between 0 and 200) of the actual tool height offset.

Tool Height: Tool height associated with the H offset selected above. This field is not editable.

Tool D Offset: Index in the offset library (between 0 and 200) of the actual tool diameter.

Tool Diameter: Tool diameter associated with the D offset selected above.

Spindle Speed: Speed at which the spindle will rotate when the spindle is started after the tool change.

Spindle Direction: Direction in which the spindle will turn after the tool change. If this is set to CW or CCW, the spindle will be started automatically after the tool change. Press F3 - Toggle or SPACE to toggle between CW, CCW, and Off.

Coolant Type: Type of coolant to activate after the tool change. If this is set to Flood or Mist, the selected coolant system will be started automatically after the tool change. Press F3 - Toggle or SPACE to toggle between Flood, Mist, and Off.

M-Series Operator’s Manual 12/20/2013 10-12

Page 96

Actual Tool Change: Determines whether an M6 code is generated (answer Yes) during the tool change. If you do not want to remove the current tool, but instead want to alter its diameter or length offsets (e.g. for doing a finish pass while using cutter compensation, you may want to use a diameter offset which is slightly larger than the actual tool for the first passes, then use the actual tool diameter for the finish pass), answer No to this question. Spindle and coolant will not be automatically turned off if you answer No here.

Press F10 - Accept, Page Up, or Page Down when you are finished to accept these values and make changes to the tool library. If you have changed any field other than the Tool Number of the Actual Tool Change field or position, you will make changes to the CNC software Tool Library. At the end of the program, Intercon always turns off the spindle and coolant and returns the Z-axis to the home position. These codes do not need to be entered at the end of your program.

F5 - Canned Cycles

appears:

When you choose the Canned Cycle operation by pressing F5 - Cycles, the following screen

M-Series Operator’s Manual 12/20/2013 10-13

Page 97

Canned Cycle Introduction #1: Using Pattern and Repeat (Drilling, boring, tapping)

Selecting F1 - Drill will give you four choices; F1 – Drill, F2 – Drill BHC, F3 – Drill Array, or F4 – Drill Repeat. F2 - Bore and F3 - Tap will have the same menu selections as drill except they will display Bore or Tap cycles

All canned cycle operations using the Drill BHC (Bolt Hole Circle) or Drill Array are identical to their equivalent using the F1 - Drill single hole selection. The use of the Drill BHC or Drill Array, however, offers the option to drill more than one hole in a pattern dictated by the new fields in the menu. F4 - Drill Repeat allows the user to repeat a set of holes with a different type drilling, boring or tapping operation with out re-entering the X, Y coordinates. The Bolt Hole Circle and array patterns are explained graphically in the following figure:

M-Series Operator’s Manual 12/20/2013 10-14

Page 98

Canned Cycle Introduction #2: Linear Repetition of Operations (Drilling, Boring, Tapping)

If you want to perform one operation several times in a linear pattern, simply define Position X, Y or both as incremental values. To do this, use the F1 – Abs/Inc Key. This key will toggle the Position value mode between incremental and absolute. If you define X and/or Y as incremental values, a new field will appear asking for the number of holes:

The numbers in the fields on the screen correspond to the following example, shown here graphically:

M-Series Operator’s Manual 12/20/2013 10-15

Page 99

Drilling (F1 in the Canned Cycle Menu: option #1)

If you press F1 - Drill from the Canned Cycle Menu, you will gain access to three types of drilling operations: Drilling, Chip Breaking, and Deep Hole drilling. The current drilling operation in use is reflected in the field “Cycle Type” and pressing F3 - Toggle or SPACE toggles between all three. In this section we will examine the first option: Drilling.

The numbers in the fields on the screen correspond to the following example, shown here graphically:

Where:

Cycle Type: Selects one of three drilling operations: Drilling, Chip Breaking, or Deep Hole drilling. Press F3 - Toggle or SPACE to toggle between the three choices.

Position: Specifies the X and Y coordinates where the drilling will take place. If either the X or Y coordinate is an incremental value, you will have the option to drill multiple holes in a linear pattern (See Canned Cycle Introduction #2).

Surface Height: Absolute Z-axis position from where each incremental depth is measured.

M-Series Operator’s Manual 12/20/2013 10-16

Page 100

Clearance Height: This parameter specifies the Z-axis height used when performing rapid moves to the position of each hole being drilled.

'Rapid To' Depth: The depth to which the cutter rapid moves before beginning to drill the hole at the specified Plunge Rate. This is below the Clearance Height but above the Surface Height.

Depth: Total: Depth of hole (incremental) as measured from Surface Height.

Plunge Rate: Z-axis speed of descent during drilling. The plunge rate can be toggled to modal, fixed or slave, this is indicated by the symbol beside the plunge rate field. If the plunge rate is modal then it will have the “M” symbol or if it is fixed it will have the “F” symbol. The slave plunge rate has no symbol and is set to the last modal plunge rate set in the program, when the modal plunge rate changes all the following slave plunge rates change until the next modal plunge rate is encountered.

Dwell Time: Delay at bottom of hole before starting ascent.

Drilling provides a rapid to the hole position at the Clearance Height, followed by a rapid Z down to the 'Rapid To' Depth. Next is a feedrate down to the specified depth. If a Spot facing cycle is desired, enter a value in the dwell time field and the cutter will wait the desired amount of time before performing a rapid move up to the Clearance Height.

Chip Breaking (F1 in the Canned Cycle Menu: option #2)

If you press F1 - Drill from the Canned Cycle Menu you will gain access to three types of drilling operations: Drilling, Chip Breaking, and Deep Hole drilling. The current drilling operation in use is reflected in the field Cycle Type, and pressing F3 - Toggle or SPACE toggles between all three. In this section we will examine the second option: Chip Breaking.

The numbers in the fields on the screen correspond to the following example, shown here graphically:

M-Series Operator’s Manual 12/20/2013 10-17